Fusion
If you're after a sheet metal flat pattern, here's one way. I've used the edge of the surface rather than a projection into a sketch as the surface edge has more accuracy. You need a small straight section at one end. See attached file.
Mark
Mark Hughes
Owner, Hughes Tooling
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Here's another version with the short flat section at the inner end of the spiral. I found editing the spiral and setting the number of rotation to a half number would cause an error. Fusion flipped the side the short line section was on. Seems like editing the spiral is OK now as long as you don't flip its direction.
Mark
Mark Hughes
Owner, Hughes Tooling
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@Design-mann2 First off, don't attach pictures, just paste them into the message or use the insert photos option.
The problem is you have chaining enabled. Just unselect, uncheck chaining then reselect.
Note. this is quite an old thread and this might now be easier using convert to sheet metal.
Mark Hughes
Owner, Hughes Tooling
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Just experimented with the convert to sheet metal option but it doesn't work with the coils\spirals Fusion creates. The problem is Fusion creates coils with the end face on a plane parallel to the coil axis not perpendicular to the helix\spiral.
Here the white line is from the center of the spiral, the orange plane is perpendicular to the spiral. Because of this error it means the thickness of coils and spirals is always wrong, the end face measures 2.5mm but the actual cross section of the coil is only 2.498 mm and this problem gets worse the corser the pitch. So the method where you create a surface then thicken is the only way to create a sheet metal spiral in Fusion.
Mark Hughes
Owner, Hughes Tooling
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@Anonymous wrote:
Hi Both,
Thanks very much for your replies, but i think 'spiral' was probably the wrong term, its more of a flat coil. Please see the attached file.
I created this in inventor and imported it in. Inventor will flat pattern it, but I can't work out how to reproduce this in Fusion.
Steve
Bit of an old post I seem to have missed. You can not create a flat pattern of this part in Fusion as the surface is twisted not just a simple bend. If you don't have inventor to unwrap this part you can export a face as a mesh to meshmixer to unwrap. then export as a SVG and reimport into Fusion. Note the SVG will need scaling by 96/72 to get the correct size.
Mark Hughes
Owner, Hughes Tooling
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Just remembered Fusion now has a thin wall extrusion option in the Solid workspace that make this a bit easier.
Attached is a new example using Thin Wall extrude then convert to sheet metal.
Mark Hughes
Owner, Hughes Tooling
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