Is it okay to connect the exposed pad to the ground pins as in the image below, or is there a recommended way to do it?
One of the most important functions of an exposed pad is heat dissipation. Good heat dissipation requires a strong connection to the ground plane.
If you're dissipating a lot of heat, this often means placing some vias within the pad. These vias must be tented (How do I define a tented via-in-pad in Eagle?) or solder will flow through the via during reflow. Check out SMSC AN18.15: PCB Design Guidelines for QFN and DQFN Packages for details on via placement and solder paste distribution for via-in-pad design. The downside to this approach is that your PCB will cost slightly more to fabricate because of the via-in-pad.
A second option is to use a topside ground pour to heatsink the chip. Connect the center pad to the ground pour through the outer ground pins and place vias in the topside ground pour to your main ground plane. See Micrel Application Hint 17: Designing P.C. Board Heat Sinks for the math on how big of a ground pour you would need. Be careful to connect enough copper to the right side of the chip for proper thermal relief or you may have soldering issues (see Eagle Quicktips: Thermal Relief).
If the chip in question isn't going to be generating significant heat, what you have right now is fine. Just make sure that the return path to your ground plane is as short as possible.
You might want to add some copper where the trace hits the ground fill - I tend to dislike 90 degree angles in PCBs. In fact I tend to prefer large fills for this purpose. I would even go so far as to completely fill in the area between the two pins shorted to ground. However this will make soldering the component somewhat more difficult due to the heat being drawn away from the pads, so it's your call. I would at least remove the 90 degree angles connecting the fill to pads and just pretty up the top one in general with some 45 degree angles, not whatever random angle that is. Just for looks.