[mplanchard]

John,

Your movie was just beautiful!

I used sheet metal for laboratory robot design for 5 years. It is light weight and accurate. A few tips on the SolidWorks design side for teams:
-Work with your Sheet metal shop to know their K-factor. SolidWorks uses .5 by default - but this is never the case. Material and shop equipment produce different values. Build these values into the initial design.

-Where do you obtain the material required for the Bend? The answer comes from the Sheet metal Flange position option. The four options are: Material Inside, Material Outside, Bend Outside and Bend from Virtual Sharp.
Material Inside: The outside edge of the Flange coincides with the fixed edge of the sheet metal feature. Material Outside: The inside edge of the Flange coincides with the fixed edge of the sheet metal feature. Bend Outside: The Flange is offset by the bend radius. Bend from Virtual Sharp: The Flange maintains the dimension to the original edge and varies the bend material condition to automatically match with the flange's end condition. Save manufacturing cost and reduce setup time.

- A sheet metal manufacturer maintains a turret of standard relief tools for Rectangular and Obround relief. Obtain the dimensions of these tools to utilize in your design.

- Alternate between 3D formed and 2D flat for every additional sheet metal feature you create. The Flatten feature alternates a sheet metal part between the flat state and formed state.

-Use interference detection in your assembly. You can create configurations of you part to test for tolerance stack up. Make certain you can get tools in to fasten hardware.

-When looking at mating pattern of holes - make certain that you are refernencing dimensions from the same edge. There may need to be a left and right version of a part if the holes are off. Marie