I designed a schematic with quite a lot of connections (88 comparators into 14 MUXes) I created ground planes on the top and bottom layers to assist with the many ground connections. I just got the PCBs from pcbway.com and I tested the ground and power connections using continuity mode on my multimeter. What I found is that the ground pins and vias with point to point connections visible on the top layer are all connected, but the ones that should have connected to the ground planes on the bottom or top layers are not connected to any other ground pin on the board. So my question is, did I do something wrong when I built the PCB design in eagle? What can I do differently to have some assurance that the board will print correctly next time? I have included links to download the schematic and the board files below.
Your board layout shows multiple unrouted nets (the yellow lines). You need to route them, otherwise your board is not a representation of your schematic.
Eagle has a feature to tell you whether you have unconnected traces. Use that! (DRC)
Generally, this system is a bit strange: you're designing a PCB, which is logical, because you want to place and connect components. Then, instead of using the components you can buy, you opt to use these Sparkfun modules that are meant for people with breadboard/veroboard instead of their own PCB design. You can save a lot of space (and money) by not doing that! Simply use the single component that's on a Sparkfun SPARKFUN-AD-MUX-16X1: that's a CD74HC4067, and it costs cents a piece, and can essentially bought at any credible electronics parts distributor (Mouser, Farnell/element14, Arrow, digikey,rs components).
Also, you've got a metric hellton of LM311 comparators. Which is fine - but there's also chips where there's multiple comparators in a single package, and that makes your job soldering things much, much easier. Also, you've forgotten to add decoupling caps to the comparators. That's a bit of a bad idea. Also, it's not very clear what purpose these comparators serve, but I trust you know what you're doing there.
What completely doesn't work is your method to generate 5V. You need a regulator. A voltage divider cannot work.
I think you need to go back to your schematic design phase and re-evaluate your component choices. Then, you need to come up with a proper way of power your board.
(also, your trace layout is pretty bad - not blaming you, if this is an autorouter result. Also, wouldn't even blame you if it wasn't: The first revision of any board I layout, I basically rip up all connections after I'm done connecting everything, and do it again, but smarter based on the things I've figured out while routing things. For example, if you're looking at your schematic, it would probably make much sense to put your comparators close to where the signals that feed into them come from, instead of all in one heap, or close to where the signals coming out of them go to.)