How to properly define BGA footprint in Eagle?
For BGA packages, you typically want the stop mask to be either slightly smaller (mask defined pad) or a tiny bit larger (copper defined pad) than the copper pad.

Eagle will automatically make the stop mask larger than the pad by a specific percentage set in the DRC of the board. This is usually much larger than you would want for a BGA.

I would advise that you disable the Stop and Cream options in the pad properties for each pad, and then manually draw a circle with a width of 0 (i.e. filled) on each of the tStop and tCream layers. This way you have full control over how bit the circles are.

The datasheet should give details of how big the mask and cream/stencil circles should be.



As a side note, for a 0.8mm pitch BGA, you may or may not be able to route between the pads, though you probably can get a single trace through the gap. Typically when wiring BGAs, you escape route them by placing a small via diagonally from the pad (not in the pad!). That way you can route the traces out on other layers.