There is a "thicken" command among the "features" commands. All you need is to select the surface, Insert > Boss/Base > Thicken, and specify the direction and thickness. Doing this may leave you with some geometry to clean up, if the intersection of the thickened spout surface goes beyond the existing kettle body geometry.
It might be cleaner to model the kettle and spout together as a non-hollow solid, and then "shell" it, though.
It depends on what type of results you are looking for. Do you want the top thickness face of the spout to be flat with the existing top thickness face of the kettle? If you only want the thickness face to be perpendicular to the spout, then knit the spout to the pink face, and use Thicken. This will give you a funky transition from the top of the kettle to the top of the spout. (the spout sheet metal is either sheered perpendicular or at an angle to the outer surface of the metal). You could fix that by placing a planar face on top of the spout and using Replace Face. Or to do it right, you would have to offset the spout to the outside, extend the top and bottom edges, create a planar face on the top and mutual trim spout, offset and planar, close up the bottom and sides of the spout with something maybe a loft. Knit it all into a solid.
And then if the bottom of the spout gets tangent to the outside of the kettle, the offset technique will not work at all.
Those are both kinda ugly. The best way to do this is to avoid mixing solid and surface techniques in thin walled parts. So just use all surface or all solid modeling.
You could write a whole chapter in a book just on this issue.
alternately, model it all as a solid with a shell and then use the "split" command.
Building on what others have suggested. - try thicken the spout surface but do not merge. Then try to use combine to ADD both bodies together. Then use Delete face to cleanup unwanted faces.
Concerning the technique for creating a spout for a jug, have you considered using the indent feature? The shape of the spout could be controlled by a tool body (boundary or loft) to deform the solid body (shell).
For more information, I have posted this technique titled Using the Indent feature to create a Spout (SolidWorks): http://www.appianwaytech.com/blog/2010/03/11/tips-and-tricks/149
If the technique helps in your specific case, let me know.
I'm curious why do you need the spout as a separate body? If the kettle is a single moulding what purpose does that serve? Only thing I can think of is if the spout is a different moulding or material from the main body? If so why not build as a single piece then use offset surface (set to zero) to extract the surfaces needed for the spout, or split the body in two after?
Speaking personally, for this kind of task I'd model it all as surfaces, knit it all up and either thicken in one hit, or cap the top surface, knit to a solid and shell. Just depends on the top finish you are after. A lot of the time I'd overbuild the top surfaces and then trim them with a curve or surface to the exact finish needed.
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