Hi,
Wondering if anyone has a suggested workflow in order to unwrap a 3D body, or even the two flat faces whereby I could then create a loft etc.
The solid is a uniform extrude of an arc, so not curved in more than one plane despite "leaning over" 10deg..
Currently I'm exporting to the component to IGES format, importing into Inventor (Trial), unwraping the surfaces, exporting to DXF, then aligning them and creating a loft to get back to a solid that's "flat"
Anyone have any ideas?
David
Does this help?
[I conjured up a body to match your description, but I might be wrong] I made a Surface Offset of the front face at 0 distance, Untrimmed external edges, Extended from edges that coincide with original body, Thickened, Split the face using original body to have the outline, added a small Extrude to one side, Converted to Sheet Metal. Now I can Unfold/Refold or make Flat Pattern:
By the way I added a hole by a simple extrusion along Y (rather perpendicular to the face) only to show that External Edge Untrim preserves internal edges.
Hamid's method is great, and something to put in the toolbox. I borrowed his model to show another approach. which is to split the body down the middle and extrude a small stationary body, I made it 1mm so you could see it, but this could be something really small like .01mm. I only did one half, but you could repeat it for the other side easily enough.
Thanks Hamid for your suggestion... I'll give it a whirl.
I've exported that component at attached.
Given it's a solid, and you will notice there are "lofted" edges between the two faces ) not actually lofts but the result of a Combine workflow ), what I might have to do is pick an origin point, use your procedure for both faces, then flatten them with SM, overlay them and create a true loft for the edges.
I'm my model there are a few of these so looking for the right workflow. The walls of the cabin in the model also have notches that intersect with other bodies. I may actually have to do my best to manufacture the part using your method, see how it fits physically in the build and then reverse engineer it slightly back into Fusion 360 for future manufacturing. I may just be pushing the tool too far.
It's easy to export to Inventor to do this operation with the native solid, but expensive for just the one feature and until I actually make one, hard to know how accurate that is also.
many thanks
David
