How to loft a hollow section

[simon.dyer]

I desire to have a tapered thickness to this cylindrical shape.
I define my profiles, and select the area I want lofted, but it fills in the entire area.

Please tell me what am I doing wrong?
https://autode.sk/2InWNWc

[jeff_strater]

You are not doing anything wrong.  This is just a limitation of the Fusion loft modeling code.  You have to do this in two steps - one for the outer boundary, one for the inner boundary, as a cut.

Give me a minute and I'll look up the forum thread where this was discussed...

[simon.dyer]

Thanks @jeff_strater
Is there a plan to remove this limitation?  Lining up the rails for the inner shape may not produce absolute accurate thickness.

[jeff_strater · Accepted solution]

here are a couple of threads.  Sometimes you can use other features to do this (Revolve).  Sometimes you can create a separate body and use Shell on that body.  But, the general solution is two lofts (one for the outer area, and another (cut) for the hollow area)

• how-to-loft-only-outer-profile-of-donut-shape
• lofting-of-hollow-features

[laughingcreek]

The other work around is to cut your profiles in half, and loft half at a time, then join together.  I've had to do that when lofting the inside shape as a cutout wasn't a good option.

[jeff_strater]

Unfortunately, we don't have such a plan right now.  I don't claim to understand the reasons, it's way down in the low-level modeler, so I understand that fixing it would be complex.  That's not to say it will never happen, it's just not high on the priority list right at the moment.

[colinNJB25]

I ran into this problem today. 😕 It seems so logical to be able to simply loft it.

[TrippyLighting]

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@colinNJB25 wrote:

I ran into this problem today. 😕 It seems so logical to be able to simply loft it.

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Yes, but it is logical to you because you don't have to deal with the math behind it 😉

[dteeter]

One option is to use a very thin plane to cut a tiny bit into the face of the two hollow items you wish to loft. Then do two lofts where each one covers 180 degrees of the two object's faces.

[kjell.verbeke]

THIS is the best answer, it saved me a load of frustration! You can even use an edge of the first loft as a rail for the second one so that your model is always closed.

[ksmith624]

I think I found a more elegant solution to the "loft a hollow section." 

1. Loft your 2 faces/profiles. The top rectangle you see highlighted is larger than the bottom rectangle. I am making an insert for a Pelican-style case for organisation purposes and I lofting the two profiles made the most sense. But I ran into the issues listed above.
2.  
3. Use the "Shell" modifier option and choose the wall thickness. 

      

[laughingcreek]

Yes,  one of the options suggested by Jeff in the fourth post. 

[Anonymous]

So this is what I did, I first made the whole non-hallow loft then I went to section analysis; made the new loft non visable then I went to sketch, showed the inner sketches of the orignal loft in the sketch tab in the browser tree lofted with the inner sketched but did a cut then hit "Ok", then go back to the browser tree and there will be a new tab called "section analysis" open the folder and delete the analysis. There you go simmalar to what you guys said.

[shahriarsifat1802164]

Hi,
Sketch on a plane and go to the loft and select the sketch and rails.
Thank you.

[therealsamchaney]

It wouldn't be hard to tell that the user is trying to create a "hollow loft". Just check if the profile selected has an enclosed region inside it. So then why not just have Fusion automatically do the proposed workaround - make a solid body from the outer profiles then make a cut with the inner profiles. All of this could happen behind the scenes. Then from the user's perspective it would be just as if Fusion actually can handle making hollow lofts. 

[TheCADWhisperer]

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@therealsamchaney wrote:

It wouldn't be hard....

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Then why does no CAD software do this in the year 2021?

[TrippyLighting]

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@therealsamchaney wrote:

It wouldn't be hard to tell that the user is trying to create a "hollow loft". 

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You are generalizing a complex problem based on the one object you've seen in this and maybe a couple of the threads. The matter is, however, you can only delay teaching users the very basics of CAD so long.

[therealsamchaney]

I'm considering this to be the most common special case of a more generalized problem. Yes, if we're talking about the most general problem - creating a loft with any number of enclosed regions within each-other - then that is much more complex and gets into a lot of topology questions. However, I don't imagine that many people would be trying to loft between two sketches that look like swiss cheese.

On the other hand, it's a pretty common case to try to loft between two profiles that each have only one enclosed region inside them, like two concentric circles for instance. Think of making custom tubing like that used in custom bicycle frames and the like. This case is pretty easy to solve as I explained in my post, and could be automated. I think it's a common enough use case for lofts that it would be worth it. There are quite a few posts asking how to do it like this one.

Even in the more generalized problem where there is more than one enclosed region in the profiles, Fusion could just prompt the user pick the pairs of enclosed regions to tell Fusion how to make the loft. This would basically be just like doing multiple lofts at once and I think could be a better workflow than making a bunch of smaller lofts.

[therealsamchaney]

At the very least, I think Fusion should better communicate that it cannot handle doing a hollow loft and give the user a warning if they select a profile with an enclosed space. As it is, Fusion allows the user to select a ring-shaped profile, and Fusion highlights it as if it's going to make the loft with the hollow center which causes the user to expect this to happen and leads to confusion when they instead get a solid body.

Instead, Fusion should show that it's actually selected the entire region including the enclosed region inside (along with the warning mentioned above) by highlighting all of it in blue. This would give the user visual feedback that they are going to end up with a solid body, not a hollow tube.

[TrippyLighting]

And you want to spend all that money end efforts in programming and software engineering to avoid having to make 2 simple, separate lofts?

While there are a good number of new users that stumble across this and then come here, I believe there is (as is often the case)  a statistically much larger number of people who manage to just test a couple of things and then simply make two lofts and move on in their work.

In general, you only have to tell a new user that once. This has been asked and answered often enough so many users now find the answer just by searching the internet.