Hi all
I'm trying to create a lofted surface between these two faces. It could also be between two of the edges if that makes things easier. It's two different sized elliptical cutouts through two cylindrical shells. Needs to be a sheet metal part so I can show a flat pattern.
Looks like the normal loft tools won't accomplish what I am aiming for. Any tips/ideas? I've attached the file below. Working with SW 2017
Thanks!
I don't see the inner surfaces as what you show
By the way, from the image in your post, you can try fill or boundary feature
You want a shape like this:
By the way, I tried to open your model first in SW2016 which caused my SW freezed and forced to shut down
I am still on 2016 so I can't open your file but could you just draw the sheet metal part and then cut it back. See my attached file
Don't do it that way.
Unfold, make the cut, then fold again.
I think I know where you are going with this Will. Perhaps you found that by using an ellipse it became dominant in the flat pattern and the rest of your holes didn't show up in the flat. If that is the case I have encountered this before and it has to be a bug in the software. What I did is was segment your ellipse and created 8 3 point arcs. Your ellipse is in the screen shot (construction) and hidden behind the new sketch geometry. Pretty close. Since it looks like, from your screenshot, you want a massive thickness I made mine 2". You may have only done that to magnify what you wanted done (far cry from .075). Not sure, but you get the idea. I have a macro somewhere to turn the ellipse into arcs but forgotten what it's called so it's pretty useless to me until I find it. It did work like a charm.
Or maybe you just wanted to try out the loft command. I did try with loft and boundary and was able to do the ellipse with both. There is an issue with a couple of the smaller holes however. I have my theories on that but don't want to get into it now.
Edit:...
Ok,, now I have egg on my face just looked at Casey's reply and I think he is on to something. He's a pretty smart fellow and follows direction much better. I Think this is what you want. Done with a sheet metal loft.
Fitting 2
Hey Dennis,
Thanks so much for taking a look at this. Your second iteration was what I was shooting for.
When you did the surface offsets, what was the purpose of those? I'm trying to follow your steps and replicate it but I can't seem to get the loft to work with the 3D sketches I've come up with.
You need a gap in the 3D sketch lines
I did the surface offsets in order to achieve something similar to your screenshot. I offset the outer surface 0" first then offset that surface 2" (just a number I came up with in order to make it look like your screenshot). When you do that the cutouts on the inside taper just like sheet metal would do when it is rolled if you made the cuts in the flat. John is correct (of course). I did leave a tiny space in each of the 3d sketches so I would have two open loops (required). I started a 3d sketc and selected the edge of the outer cutout an converted. Ended the 3d sketch and started another 3d sketch on the inner surface edge, converted ended the sketch then inserted the gap in each.
You may have noticed that there is a tiny (very tiny) gap in the top of each 3d sketch you probably missed when you did the sketch offset. To get around this I made each curve a fit spline. Kinda the lazy man's approach but may (probably is the way to go.
Fit spline...awesome. That worked. Thanks so much for your help
Did you try creating guide lines for the loft? A couple of guidelines could help a lot.
Another option is to do a lofted cut AFTER it is a solid. That way, your walls are created for you.
Sometimes Solidworks forces you to try different ways to skin your cat.