Long answer: You would have to start from scratch and create a forming tool that will do that shape. Or slice it up and create a lofted bend. Use that part as a reference, but theres not much you can do about converting it to sheetmetal.
In 2011 there is a convert to sheet metal command.
But I have to be honest. I tried it and it is struggling with your part.
I even tried creating a converted entity of the edge with no luck. Tried drawing a spline a long that edge and I got this message
when attempting to extrude as a sheet metal part. I am pretty sure in saying that sheet metal will struggle and not convert
irregular shapes such as curves and splines.
Your shape is built from splines with the metal being drawn in places.
SolidWorks needs entities based on radii and straight line segments that can be wrapped. If the metal is drawn (stretched or compressed) SolidWorks can't flatten it.
SolidWorks sheetmetal is for parts that you can create on a brake press, or simple bends and wipes in a progressive die.
You would need a program such as BlankWorks or LogoPress to flatten this part.
Good morning Sergio,
Yes you can bend this shape using SW.
How it is done;
1. I inserted your part in an assembly
2. then added a new part called "Test-ahh" (I just picked a plane to insert the new part)
3. Start a 3D sketch
4. Convert the entities on one side of your part
5. Start another sketch
6. Convert the entities on the second side of your part (you can't do both spline edges on one sketch)
7. Come out of both sketches
8. Use the Loft Bend tool
9. Now you can flatten the part, but good luck finding a machine to form it
Test-ahh.SLDPRT.zip 199.3 K