I can't open your file, still on 2010, but nobody eles has piped up so I will give it a try.
Sweep is probably my least favorite feature. It promises so much and delivers so badly. You might try making three separate sweeps, one up each long side and then one at the tip. Or try two sweeps for the long sides and then use a Loft or Boundary Surface for the tip.
As far as the Thicken problem goes, check the part for radius of curvature. You will probably find some areas with less than expected values. Cleaning up the Sweep may get rid of the bad areas.
The odd geometry at the tip of your part is caused by the fact that your sweep profile sketch is not perpendicular to the sweep path at the point of your sketch plane. To fix this, you can create a plane at the end of your 3D sketch (3DSketch17) and use that plane for your profile sketch. This will keep the sketch perpendicular as it follows the path.
As for the thickening issue ... Jerry is correct, it is usually related to the radius size. A part with very simple geometry will often thicken with radii smaller than the thickness but as the geometry gets more complex the small radii will cause problems. You could make the sweep without the radius along the top edge and then add it after the thicken.
Thanks for the responses Jerry and Keith!
I got it working by taking some of the advice you provided.
For anyone else that is looking for a fix for a similar issue I will quickly explain what I did to get it working:
Instead of doing one sweep around the whole suface, I took Jerrys advice and did 2 seperate surface sweeps (one on each side). I used the loft command to connect the two, however this did not fix the thickening issue.
The main problems with the thickening were the top loft surface and the areas where the side sweeps connected to the main hub. As noted, the thicken could not resolve due to the small radii along these edges. To avoid this problem, instead of knitting the whole part together, I performed 3 seperate thickens: 1 on the main body and 1 for each side sweep. I then connected the 3 resulting solids with the combine feature. The final top loft was then added to the already thicken parts using the standard loft command.
Thanks again for the help!