Really you can't loft ring to ring??

[Anonymous]

If i wanna loft a ring sketch (30 diam , 20 inner diam to a higher(say 20) ring sketch ( 20 diam , 10 inner diam)

fusion can't do that ??? why???

It wants me to go through and take massive time make full shapes before you can complete a simple loft.???

[jhackney1972]

i assume you are working in millimeters, you did not specify.  You also did not specify how far apart the rings were but you can change the model if you want something different.  You should attach your model so the forum users can help you understand what you are doing wrong, not blame your problems on Fusion 360.  By the way, this can be created with any number of different methods, loft is just one of them.  My model is attached.

[TrippyLighting]

That's correct. You cannot create hollow lofts in Fusion 360. There are numerous ways to approach that, none of which are too time consuming.

[jeff_strater]

I don't pretend to understand the math involved, but the answer is:  this is just a limitation of the loft algorithm.  All you really have to do is create two lofts, one as a solid for the outer shape, and a cut loft for the inner shape.  Not really all that burdensome, IMO

[steven_zhuQDRBU]

You can also do it a more complex(but cool) way: Go to surface, create, then loft the inner rings of sketch 1 and 2 together. Then loft the outer rings of sketch 1 and 2. Now go to surface, create, then patch the space in between the outer and inner circles for each side of the shape. Now the shape is enclosed(but it is still a surface body), you can go to modify, stitch. Make sure you stitch every single face(4 faces in total. Inner face, outer face, both rings). Now you should be left with a solid body.

[steven_zhuQDRBU]

The completed loft:

[charles.scheidecker]

That was exactly the solution I needed, thank you!

[Jalapeno311]

This is awesome, you just loft the ring and then do a second loft delete of the inside. Thank you!

[Jalapeno311]

This is awesome and so easy, you just lofted the ring and then did a second loft on the inter circle delete. Thank you!

[TheCADWhisperer]

@Jalapeno311 

Shell might be even easier

Revolve would work easily too.

[Jalapeno311]

Thank you!! I’m still learning a ton in fusion. It’s a connection part/tube
I made with different sizes on either end. The double loft seemed to work
and it printed nicely. I’ll try the shell method too. I have had problems
where I need inside spec on one side and outside spec on the other that
caused me problems.

Mike Stringer
Innovation Specialist
Pine Crest School - Fort Lauderdale Campus
954-492-4100| www.pinecrest.edu