This part is an IGES file that is included in the SolidWorks 2007 Sheet Metal Training Manual as one of the examples on how to convert an imported (dumb) part to sheet metal.

According to the explanations in the manual, this can be done as a two step process, by first using the Rip feature to select edges or corners that will be cut with a small gap in order to allow the part to be flattened as a sheet metal part, and then adding bends using the Insert Bends feature.  Or it can be done in only one step, selecting Insert Bends to recognize the bends in the part and rip corners at the same time. In this image, Face 1, the fixed face, is the bottom rectangular face of the part, the edges highlighted in blue are those that will be ripped, and are listed under Rip Parameters, together with the gap value of 0.5 mm. Other options are also available, such as changing the bending radio or auto relief.

The result is a sheet metal part, with rips and bends that have been added to it and that we can select and edit separately through the feature manager.  Notice that the sharp corners in the original part were converted into sharp bends using the default bend radius value, while the existing bends, like that tab on the right, were converted into round bends, using their current radii.

The flattened sheet metal part looks like this.

So I tried doing the same using the new SW2009 feature, Convert to Sheet metal, but I’m afraid my results were not all that good. 

I tried making similar choices to those I made before, in order to achieve the same results. For the fixed face, I chose the same as before, the bottom rectangular face.  Hard as I tried, SW would not allow me to choose the edges to be ripped in this case, so I chose the edges that represented bends instead (in pink), and SW identified the edges to be ripped (in purple). I chose the same bending radio and the same gap as before.

At this point, everything seemed to be going exactly the same as when using Insert Bends, but then I noticed something. It’s kind of hard to see while looking at the isometric view, because the part is made semi-transparent, but notice how, as you choose your edges, a preview of what your converted sheet metal part will look like appears on the screen, in a yellowish color. Notice that everything in the part seems to be included already, except for one thing: that little tab on the right.  Can you see it?  The tab is not colored yellow like the rest of the part, which means it will not be included in the sheet metal part.

Why is this? Well, I think the bend hasn’t been recognized. So, I tried the button that says Collect All Bends, but got a message saying that no previous bends had been made. I also tried selecting the edge in the part, but got a message saying that this could not be a bend edge since there was a face for this edge that is not planar. So, without any more ideas on how to make SW recognize this bend, this is what results from using the new SW2009 feature on this particular IGES file. The tab is gone and we only have sharp bend features added to the feature manager, but no round bends like in the previous example.

So, I guess the new feature isn’t really the tool to use for these particular kinds of parts. I do wish there were a few more examples of the uses and limitations of the SW2009 Convert to Sheet Metal feature, especially for those of us that are just learning about sheet metal altogether.