Is it possible to combine a loft and a sweep?

[eselick]

Hi - I'm a beginner so have mercy :)) As the screen cast explains I've swept a profile around an arc and then I need to use loft to modify the last part of the sweep. Any help will be appreciated.

Thanks

Here's the screencast. 

[davebYYPCU]

Lofting to an edge profile is the limitation, 

Use a Surface Loft, to cut the top away,

Select these two lines as profiles, and

this one as a centre line rail.

Use Split body, and the new surface loft as the cutter for the split, and remove the offcut body

Might help...

[eselick]

How do I select "lines" to use as the profile? When I hover the mouse over the lines you indicated and click I get the following.

[TheCADWhisperer]

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

[chrisplyler]

To select LINES as inputs for a Loft, you must use Surface>Create>Loft instead of Solid>Create>Loft.

In the Solid workspace, the Create tools need PROFILES as inputs, because it takes an AREA to turn into a 3D VOLUME.

In the Surface workspace, the Create tools need LINES (or edges) as inputs, because that's what it takes to produce a 2D surface area.

[eselick]

I'm attaching my model. Thanks for the clarification about using surface loft. With surface loft I'm getting the message "rail is missing profiles":

[chrisplyler]

Use the Centerline guide type instead of the Rail guide type.

[eselick]

Redid the surface loft with centerline and got this which doesn't appear correct since the outer curve looks like it's being cut off:

I just tried using rails again with the small inner arc selected. This touches both profiles.

It seems to work and gives this

:

[chrisplyler]

Ahhh... good thinking.

[eselick · Accepted solution]

In surface mode I've managed to split away the extra faces (splitting body didn't work) and I get this which is more or less what I wanted:

The last image shows the filleted edge. It's not quite right but - it's good enough for now. Thanks everyone.. 

 

[JamieGilchrist]

Hi @eselick ,

Here's another approach that I think get's you where you want to be.  So I first focused on the part that you want the truncation to happen and use a revolve to get the quarter pie shape.

Next I made to sketch that represents the "bottom" of your truncation

Then made this lofted surface (main body visibility is toggled off here)

Split the revolved body using that surface (Extend splitting tools on) 

Next was another revolve to get the other part of your main shape that isn't truncated and one more revolve to get the "scalloped cut" in the middle

I've attached my model so you can see how I approached this.