I was able to model the lug as follows-
First I extruded the lug sideways but as a drawing twice as thick as I wanted the final lug. I drew the lug profile with a 180 arc at the end of it so that the cylindrical curve at the end would already be there.
Then I drew a top profile to cut the lug to the curving taper toward the end.
Then I put a uniform chamfer along the outer edge, around the rounded end.
At this point I looked at the side sketch plane and could see the line segments between the section of the chamfer that was a smoothly curved plane, and the section that was conical at the end of the lug. i carefully drew two lines on the plane that aligned exactly with these segments defining the conical section and made those into a sketch that encompassed the conical end of the side profile of the lug.
I used this profile to separate the rounded and partly conical tip from the rest of the lug as a separate body.
I now had the basic lug- with the tip of the lug separate, in the form of a half cylinder, and half cone- and an even chamfer running continuously from the main body of the lug and onto the part I separated.
Now you do the trick of rotating the chamfer… except you select both the top edge chamfer, and the now separate conical chamfer. And then invoke the rotate tool and rotate the chamfer enough to get the taper to a point on the top edge but not run out of room on the conical edge.
You will find that the Z axis rotation might give a smoother result.
Once I did that, I unioned the two pieces of the lug, and then I cut off the bottom ( that extra thickness i initially extruded so I could get a good conic section ) to match the final curve of the bottom of the lug and expose just a little over half of the cylindrical/conic bend at the end of the lug.