Flatten cylinder in SE 14?

[jlcochran1]

How do you flatten a cylinder in SE 14. I would like to take the shell of a vessel, complete with holes for nozzles and unroll, save as .dxf for burn table output. In Inventor you pick the inside surface of the cylinder, SolidWorks an edge. In SE how do I make the cut in the protruded cylinder such that it will let me pick an edge to flatten?

 

[fwc]

You can do this in sheet metal environment.
Click the “Contour Flange” icon then use the “Arc by Center” to create the arc. The arc angle should be slightly less than 360 degrees and ensure that the gap is not closed by the thickness of the material when defining the material side.
After creating this you can add features onwards.
You can then flatten the part in Model > Flat Pattern by selecting the edge.
Hope this helps.

 

[jlcochran1]

If I understand you correctly you cannot convert a protusion to a sheet metal part after the fact for unfolding, you must create it in sheet metal environment? How would you create and unfold a conical section? There seem to be significant differences in how Inventor, SW and SE approach sheet metal.

 

[rollacrc]

YES you are correct you have to create it in the sheet metal environment. to make a conical shape you would have to draw 2 sketchs and use the lofted flange command..to be real honest i haven't had good luck getting them to turn out you have to leave the gap just like fwc said for your cyl. if there is a better way i sure would like to know ...

 

[fwc]

Try this,
1. Draw the first arc then draw a construction line from one of the arc end to the arc centre then from the arc centre to the other arc end. This will form a V-shape.
2. Create the second arc using parallel plane.
3. When creating the second arc (try with a smaller arc), make sure that the second arc centre is concentric with the first arc and connect the two arc ends to the Construction lines i.e. the V-shape.
4. Now try using the Lofted Flange.