1. Show all pins.
This is the most specific, leaving nothing ambiguous or, God forbid, hidden, on the schematic.
Remember, the schematic is a document. A language. It conveys information. Hide as little as possible! Do not make it a challenge for the reader to figure out what you're doing!
2. Use a normal symbol, and a modified footprint (renumber pads so they get set to the same net).
This requires duplicates of some footprints, but is one of the slickest compromises between what-you-say and what-you-do. It's not at all unreasonable for SOT-89 and SOT-223 parts (where the tab is almost always physically connected, at the surface or in the lead frame).
3. Hide pins and connect them up manually.
This is the greatest risk for making a mistake, in the first place just because it's tiresome to do in Altium, and subsequently because you need to set each pin on each copy of each part that this is done on. It's so bad, I suspect it's a case of: "well, we'll allow you to screw this up, but you're doing it at your own peril."
4. Set the pins to multiple pads in the footprint editor. (Lie)
Sadly, Altium does not have this feature. It's been requested basically since AD came out. Others have it (even Multisim / Ultiboard has one-to-many pin mapping). Still, nothing... (Well, unless they're addressing it in v17 or 18, I don't know. Seems doubtful.)
5. Set the hidden pins to additional nets.
This isn't directly applicable, but on a related note: you can set hidden pins to an arbitrary net name, then place that net name on the schematic elsewhere (with a Net Label) and connect to it, or apply a class or rule or whatever.
Tim