difficulties lofting and patching an awkward shape

[maker9876]

I would like to create a LOFT from the bottom rectangular prolile, through the rectangle above it, following the rails that curve up to the right, and then finally to include a profile generated from the 3 orthoganal lines in the top plane and the conic curve that is in the vertical plane.

Then afterwards would wish to patch the top and bottom of the structure to create a solid, in which will then create a couple of holes before 3d printing.

Am in the PATCH environment but cannot get this to work.

In particular can't get the top curved plane to be recognised as a profile. The curved line is considered to not be continuous with the orthoganal lines.

Any suggestions how to tackle this problem much appreciated.

[jakefowler · Accepted solution]

Hi maker9876, 

Welcome to the Fusion 360 community, and many thanks for your post!

A couple of suggestions that might help with this model:

• If you disable the Chain Selection checkbox in the Loft dialog, you will be able to pick individual edges and chain them together manually into profiles/rails. This might help in selecting the non-planar profile at the top.
• If you're still having trouble creating the loft (I made a simple recreation of your sketch network, and actually wasn't able to generate a result using the non-planar profile), you could approach this by lofting each side of the shape individually. Below is a quick video showing what I mean: deselect Chain Selection, and pick just the edges that represent one side of your solid. You'll probably need to use the New Input button when selecting the rails to avoid them becoming merged with the previously-selected profiles. 

• OK the command, and start another Patch loft. Repeat this for each side of the model until you've enclosed the volume. Then open the Stitch command (from the Modify menu in the Patch workspace), select all of your loft surfaces, and you should be able to stitch these into a solid body

If you get stuck, or need more info, let me know and I can put together a more detailed video of this workflow.

Hope this helps!

Jake

[keqingsong]

@maker9876 , did this resolve your issue? 

[maker9876]

Many thanks Jake. Impressed by how easy you make it look. Today I'll be at the Fablab and will play with this some more. Last week I built something similar by carving out solids. The top curved plane was easy to achieve by splitting a solid. Are there any simple rules before one gets started that will dictate whether solids or surfaces are going to be more appropriate?

[jakefowler]

Hi maker9876,

Glad that helped!

The Model and Patch Loft commands are essentially using the same technology underneath, so there shouldn't be huge differences in behaviour. But solid loft only accepts planar sketch profiles (although it does accept non-planar model faces). If you're using planar profiles, or you're lofting between faces on existing solid volumes, I'd use solid loft simply because it's more efficient. Surface loft takes more work to form a solid volume, but the advantage of building the shape face-by-face is that it gives you more flexiblility to work with complex/non-planar profiles.

And certainly don't blame you for hitting difficulties with Loft: we recognise that the interface isn't all that intuitive at the moment. In fact, we have a brand new UI in the works, which will provide tables for managing the profiles and rails. This should be with you in an update coming later in the month. Here's a sneak peek of the in-dev functionality:

We're hoping this will make the tool much more straightforward to use 🙂

If you had any further queries or this didn't answer your question fully, do let us know.

Thanks!

Jake

[cekuhnen]

@jakefowler Ah nice to see that the Loft etc dialogs finally get a better UI 😉

[Anonymous]

Really good to know to hold off a bit more on some things like that in producing educational content. 🙂

Jesse