How do I edit thermals on pads in Eagle?
Eagle will only do 4-contact thermals, and only with horizontal/vertical connections.

However, you can increase the width of the connecting traces (thereby shrinking the gaps) by modifying the Width setting of the polygon you are connecting to.  This doesn't require making changes to the component library.

For high-current connections I generally make the width equal to the drill diameter.  This provides enough copper to match the surface area of plated hole interface, but still provides some cutouts to improve solderability.

Of course, any thermals will limit current flow for the same reason they limit heat flow.  It's a design decision on how much copper to relieve, whether using two, four, or eight connections.

If you change the width of the polygon it will effect the rest of that polygon's thermals and borders.  If this doesn't work in your design, you can make two overlapping polygons: one around your high-current plated through hole and the other over the rest of your filled area.  Give them the same net name and the same priority setting, and let them overlap a bit.  Then you can change the width of the polygon in question and leave the other one as-is.