If you have a tube designed in CAD, the easy way to grind it to the shape that you want is to unfold the tube in CAD, print it out, tape it to the tube, and grind away.
Unfolding tubes in Solidworks is pretty easy. First, make a reference axis on the tube concentric to the tube, and create a reference plane that is coincident to that axis (you will have to pick another reference point, but this is arbitrary, so I usually just pick the origin).
Next, create a sketch on the plane that you created, and create a line through the axis that is longer than the tube. Do an extruded cut, thin feature, with a very small cut thickness (0.001").
Your tube will now have a thin slit in it, and now we can use Solidworks to convert the tube into sheet metal. Go to Insert -> Sheet Metal -> Bends and change the radius to the radius of the tube, and K-factor to 1.
Select the
inside edge of one of your cut lines and hit okay. Your tube should now be converted to sheet metal. The last thing you need to do is right click on the tube and click Flatten. Your tube should now be flat. (Alternatively, you can insert an unfold feature under the sheet metal menu).
Make a drawing from the part in 1:1 scale, print, cut, and wrap it around the tube.
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