The traces on the Teensy 3.5 & 3.6 PCB are 5 mils (0.127 mm) wide in the BGA area, and 7 mils (0.178 mm) on the rest of the board. Most of the traces on the bottom layer are 8 mils (0.203 mm). Most power is routed as planes on layers 2 and 5, but a few power traces on the internal layers are 10 to 15 mils wide.
The vias inside the BGA area are 19.2 mils (0.488 mm) diameter, and the vias on the rest of the board are 25 mils diameter. The BGA pads are 0.5 mm diameter. The vias have a staggered offset relative to the BGA pads, only 34.3 mil (0.874 mm) apart between even numbered rows and 44.4 mil (1.128 mm) apart between odd numbered rows. This staggered arrangements allows 50% more horizontal routing. One horizontal trace can still pass between the 34.3 mil spaced vias on the internal layers, but on every other BGA row, two traces can pass between the 44.4 mil spaced vias. You probably would not need this trick for a normal PCB design where traces can escape from the BGA in all 4 directions, but it's pretty much essential to achieving the escape routing on the limited area of the Teensy 3.5 & 3.6 layout.
While I used 0.5 mm diameter pads, apparently going down to at little as 0.4 mm is acceptable. But smaller geometry pads do require different manufacturing steps to build the boards.