Are thin connections between ground planes "islands" acceptable for ~0.5mA?
Here's some general advice which may or may not be applicable to your circuit.


Interference pickup. One of the functions of a ground plane is to shield interference from other parts of the circuit, and the outside world. If you have a really large piece of ground plane which is connected only through a small track like that, the big plane  may act as an antenna an pick up interference which might disturb the operation of the op amp. I would not suspect this to be the case in your layout, though.

Length to the capacitor. The point of having a local capacitor near a a chip (C2 in this case) is to absorb fast current spikes without being hindered by stray inductance. But what you need to take into account isn't just the length to Vcc, but the total loop length from the negative supply pin to the capacitor to Vcc. You may want to consider moving the capacitor to the bottom of the chip and move the chip up a bit. Probably not a problem in your case, but something to keep in mind. 
Before worrying about small stretches of thin tracks, you may want to beef up those anemic Vcc tracks. You could easily double, or more, the track width of Vcc, across the whole board. Once again not necessarily a problem but good practice. After all, the small stretch of ground track you're pointing to would not contribute much to lowering the total series resistance.
Changes in ground fill properties, or changes made by a careless board house. You have routed a track through the gap, which is good. The ground plane pour would not have filled that gap as you can see between pins 3 and 4. But even if it did, but you later changed the ground plane isolation distance, it might have ended up breaking the connection. Likewise, a careless board house could trim away that track, assuming it was just unnecessary ground fill and it would be better for manufacturing tolerances to remove it. Such things have happened "in real life" and should be considered.