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.
hello, I see the examples given here, but I have a part that needs a flange built from a curved edge. Inventor doesn't like curved edges for a flange- any suggestions for this flat pattern guide?
Allen, I'm brand new to Inventor and I was wondering if you found any great tutorials that helped you find the solution to your problem. I will be working with a lot of twisted sheet metal (laser cut) and need to learn the right way to create the sketches. Also, you didn't post the "solution" file in your success post and, if you can share it, that would be great so we can see how you solved the problem. Thanks!
Attached is the solution for this part, A01.
I can't put my hands on any tutorials at the moment, but I'm sure there are some out there. I've learned a lot just by keeping an eye on this forum.
Part A01 is one panel of an assembly the wraps a steel column. I made a surface model to represent the skin of the finished assembly. The surface is then derived into a part file, A01, and trimmed down to desired size of the finished panel. To make this panel I used sheet metal loft. The loft sketches are drawn using the projected edges of the trimmed surface. Projected edges alone can't be used for lofting. As someone here suggested, I had to draw new sketch lines constrained to the projected edges, then use those for the loft command. That was the solution to my problem.
The sweet thing about this method is that I can make the next panel by saving A01 as a new part, then redefine the surface trim by simply moving the workplanes. (The surface is trimmed to these planes, and the loft sketches are drawn on them as well.)
Hope this helps.