Machine designers will LOVE the new Belt/Chain features in SolidWorks 2007.  The days of sketching arcs and lines to simulate a belt could be over for most users with the new features that have been added.

Two Belt/Chain Features have been added.  One feature allows you to simulate a belt in a 2D sketch environment and the other allows you to simulate or create a belt part in a 3D Assembly.  Lets start with the 2D feature.

To use the Belt/Chain feature in the 2D environment, all of the sketched pulleys must be individual sketch blocks.  You have the option to constrain the blocks using sketch relations and dimensions.  Selecting Belt/Chain from the Tools->Sketch Entities menu pulls up a Property Manager for the feature.  Selecting the sketch pulleys one by one yields a dynamic preview of the belt with each additional pulley selected.  Once all sketch pulleys are selected, you can use the direction arrows on the screen to change the direction wrap of the belt on each pulley.  Further examination of the Property Manager shows additional options that can be very useful.

The belt length based on your selection is shown.  Based on this data, you change the Belt Length options to “Driven” to match available off the shelf belt lengths.  To make this work, you will need to have one “adjuster” pulley unconstrained in a single direction.  By changing the option to driven, the sketch will automatically move the pulley to the proper position once you select “OK” to close the command.  By default, the “Engage Belt” option is checked.  With this option, you can rotate one pulley in the sketch and ALL the other pulleys rotate the proper amount!  The figure to the right shows the pulleys rotated a few degrees (note the vertical lines from the center of each block).

The Assembly Belt feature works in a very similar manner.  It can be found under the Insert->Assembly Features menu.  You can select cylindrical faces of each pulley or an axis to designate the belt path (selecting an axis requires you to manually set the diameter of the pulley).  Just like the sketch feature, you can select direction arrows on each pulley to change the belt path.  You can also set the belt length to be driven (as with the sketch feature you will need to have one pulley component left unconstrained).

You can also designate the belt thickness.  This is particularly useful with another option available which is the “Create belt part” checkbox.  With this option selected, SolidWorks will create an in-context part file containing a derived sketch of the belt path.  You can then open this part file and create an Extrude feature to complete the belt.  As with the sketch Belt/Chain feature, you can choose the “Engage belt” option which allows you to rotate all the pulleys by rotating a single pulley in the chain.

That’s all for now….more reviews to come soon.