I'm not sure where I was failing before. After reading some links I found by searching "net_short" in COS and playing around a bit, I was able to implement NET_SHORT either from the schematic or the board. My demo project was quick and simple, thus omitting hierarchical blocks and other project bits that might ultimately end up causing problems. I'm going to play more...
Place any single-pin comp on the schematic and connect it to some net. Then click on the pin (not the comp body!), which lights up a flashing red box around the pin for me, and open the Attributes form. Add a new prop to the pin, name it NET_SHORT, and put the nets, separated by a colon, as the prop value. Without having to specifically set up this property to transfer in PXL, but with "Create user-defined properties" checked on the Export Physical form (which I always check), the prop shows up on pins in Allegro.
Imagine the pin has "direct" connection to NET1 and the prop is NET_SHORT=NET1:NET2. Routing to NET1 is like normal. But when I route NET2 to the pin, it doesn't want to add the connection because a DRC error is being created. But if I pick Done from the RMB menu, I believe the DRC error is being suppressed.
This does in fact work, but it's not exactly intuitive since the "additional" Clines don't really want to join the pin, you can to make them. Furthermore, adding the prop to the schematic pin by hand is archaic.
I can simply connect a single-pin comp to any single net and run PXL. In Allegro, I manually add the same prop to the pin. In this case, again, routing the "direct" Cline is easy but I still get a DRC error when I drop in the "additional" Clines. Until I noticed that I must avoid bringing the "additional" Clines to the origin of the pin and just end them somewhere within the area of the pad. Also, I can't route from the pin with the NET_SHORT property because the Cline will then get a "Dummy net" connection and I can't create connectivity with elements of the "additional" net. Shapes are easy.
I could rip out a PCB SKILL program to easily allow users to select nets and apply this property, maybe even with some intelligence to assist users or auto-pick for them. So that's a possible plus, although I think I need to ponder how a tool for doing this with a GUI could be best used. Since Concept SKILL doesn't support native forms, it's far more difficult to try something similar on the front end, where it belongs.
So again, it works. But I still have to manually type in the net names (but not the property). And I have to route towards the pin with the NET_SHORT property and be careful to end the Cline on some random spot within the finish pad area. Plus there's no schematic annotation of shorted nets
Either method has serious drawbacks. I can understand why this was a User Group Top 10 request as stated by Solution ID 1835116, but I'd bet the user group had a less clumsy implementation in mind.
Please, someone tell me I've still got it wrong and there's a sensible way to short nets at a specific point on the board.