CadSoft Eagle polygon won't reach pads in Molex library
I found the Molex 5569 library you're using. Whoever made this library did something very odd. For each square through-hole pad, they also added a co-centric hole on top of it. So there's a pad and a hole in the same spot for every pin. Eagle is programmed to isolate pours away from holes, which is why you're getting an isolation circle around each square pad. I can't think of a reason the author of this library would have done it that way. It's certainly not necessary to put a hole on top of a through-hole pad.

To fix this, open the Molex library and open the package that corresponds to the part you're using. If you want to be thorough, do this to every package in the library. Go to each pad and delete the hole that is co-centric with every single pad. You'll hardly notice the difference visually, but you can see it in the image below. The pad on the left has had the offending hole deleted. The pad on the right still has the hole.



As a last step, go back to your PCB layout and click Library->Update All. The pour should now engage each pad. In the example image below, I removed the hole from just the first pin and connected it to a pour.