Help me extend a loft?

Try making it as a surface to start instead of a solid.  Make a surface loft of the 2 cross-sections, then you can extend that to the end surface.  It should continue the curvatures neatly.  Then make a solid out of the complete surface.

here is one option. i deleted the end face of the loft. and then extended the sufaces past where you needed. trimmed them with the plane. used a fill surface to close it back up and make it a solid. and lastly combined the 2 solids.

Looks like there's a non-tangent edge in one of your sketches.  This is probably creating self-intersecting geometry (or a singularity) causing the surface extend to fail.  Here's what I got after correcting the non-tangent edge.  By the way, I'm not a surfacing expert; having just taken the class a couple of weeks ago, I'm just beginning to dabble in this interesting area of modeling.

I was able to do with lofting, see if this works for you.

O.k., it appears that the small straight line between the arcs in your loft profiles are causing the problem, and this makes sense if you think about it.  The small flat on Sketch22 is about .005" long, the small flat on Sketch20 is about .001" long, when we are extending the surface we are further reducing the length of this small line, eventually to the point where it becomes non-existent and the corresponding arc geometry self-intersects (at least this is what it looks like from my perspective).  What I did in the attached model was to create a fit spline between the two arc sections and the small straight line in each sketch profile, this may or may not be acceptable to you however, it does eliminate any self intersections created from using the extend surface command.  This is just a guess on my part, maybe someone else will chime in if I'm wrong on my thinking.