Trouble Creating a Shell with a Loft

[apabst]

I'm trying to model a boot using a series of lofts to create the ankle to knee area. After making my sketch profiles and trying to create a loft from them I receive the following errors:

Error:   The loft could not be created.
    Try changing the inputs, swapping profiles for rails or a centerline, or adjusting the continuity conditions.
Error: Tool body creation failed

The shapes that I'm defining for each profile are not terribly complex, so I'm not sure why this would be happening. I've watched a number of tutorials and read a number articles, but can't seem to find a solution.

Does anyone have any ideas as to how I could get this to work?

[etfrench]

It worked for me after using the top of the boot to create a new sketch.

Extruding the top of the boot also fails. 

[TrippyLighting · Accepted solution]

Creating hollow lofts in one go is not possible, or at least it's been reported not to work several times.

Using a projected sketch of existing geometry as the start for the loft will not provide you with the "smooth" or "tangency" start condition which would allow for a smooth transition between the existing geometry and the new loft.

You can approach this several ways. If you created a shell on the existing geometry, then simply roll the timeline back to before the shell operation and then create a solid loft.

The now subsequent shell operation will likely turn yellow afterwards as it looses the reference surface you picked previously to defining the shell. Simply edit the shell operation and pick the new top surface of your geometry.

You could also create 2 separate lofts in the patch environment, one for the inner and one for the outer surface. then you can cap both ends, stitch them into a solid and combine-join the result with the existing geometry.

[Anonymous]

Hi All 

I see this is an old post, but I came up with another way, if anyone else might come across this page through a web search, as I did.

I also wanted to transition from a square box perimeter shape to a round hose inlet, made 5mm offsets to each side of the respective sketches, selected the "shell" surfaces, and expected it to produce a hollow Loft shape. But i also got this error. 

So what I did was remove the offsets from my sketches and it created a solid loft. I chose profile "tangent" direction, it just gives a more pleasing curve.

Then i hid the loft body, on the eye icon, went back to the sketches, put back the offsets on -5mm of the original geometry, and created another loft with the inner offset surface. NOW, when it gives the preview, I switched the previous loft body back on, But choose Cut, on the operation. This then subtracts the inner volume from the previous loft, leaving you with a outer shell loft intersection.

Attached is the pictures of what i mean. Hopes this helps somebody.

[csy528]

Hi, I've just tried your method and it's absolutely genius and very helpful. Thank you!!!