I know Inventor doesn't like curved sheet metal, especially compound curves, and I understand that. Curved dies in a brake press aint exactly the norm :-) .
Attached is a sheet metal part with a curved/twisted face. It blends into a flat face and then another curved face on one side which works out just fine. The other side is a slanted flat face with a bend joining the curved face. Therein lies
the problem. I can't put a true bend along this edge because it's twisted. Normally, when working with curved faces, if you can manage to make a small flat space tangent to the edge of the curve you can use that to add a bend feature.
But the attached part, A01, is not cooperating. After about 10 hours of fussing with this thing, I have managed to attach the curved face to the slanted face by using splines to make the transition. But it still won't fully flatten - it's not a true bend.
Please, does anyone have an idea how to put a bend on this corner so it will flatten?
Inventor 2013 64bit, Windows 7
Solved! Go to Solution.
What is the tolerance on your part?
The attached example might give you some ideas.
The lofted flange was the very first thing I tried. Made my two sketches using just the projected edges of my surface model, but the loft command wouldn't let me select the large curve portion of the sketches. After looking at your example I gave it another try. Same result. Then I converted the projected lines into construction lines and traced over them with new lines/arcs. The loft command will now let me select the entire sketch, but it still won't complete the command. Tried with and without the bend radii in the sketch.
Since it wont loft it all in one go, I think I'll try breaking it up into multiple lofts.
Have a look at the attached (2013). It looks like JDMather beat me to it with a lofted flange approach, but this might be worth a look as well.
For what it's worth, I'd suggest cleaning up your sketches a bit. You might have noticed that both JDMather and I started fresh with new sketches. One quick way to simplify: If you parts are symmetrical (as it appears you intend), you only need to sketch one side, then you can derive/mirror to create the opposite side. I've atached two example methods of this workflow. I'd recommend this whether you use my (surface/thicken) approach or Mr. Mather's lofted flange.
Good luck, and let me know if you have any questions about my approach or recommendations.
Then I converted the projected lines into construction lines and traced over them with new lines/arcs.
The lines and arcs must have Tangent constraints.
Maybe start a new sketch and use the construction lines from the projected sketch for eyeball reference only.
Use logical dimensions and then compare this sketch to the projected construction sketch to check deviation. If the deviation is within your manufacturing tolerance......
Thanks, guys, for your tips.
Sketching new Tangent Arcs did the trick. Gotta check my master sketches now - they must have lost some constraints. At least I now know this thing does work.
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