Use a ground pour, not traces for ground - this makes a better ground, and greatly eases routing. Use the polygon tool to draw the outline of the pour (eagle will handle clearance from holes, traces, and board edges), and then click one of the edges with the name tool and change it to the name of your ground net (which you should name GND, but probably haven't because you say this is your first PCB)Where is power coming in? How is it supplied? Be particularly careful when powering something from automotive 12v supply, as the voltage on it can be significantly higher than 12v when the battery is fully charged, and it is notoriously noisy, with large spikes.
Wiring on the red activity LED is wrong too.Don't level shift it, and CS is active low, so you want the negative side of the LED connected to CS before the level shifter, through a 1k resistor, with other end tied to 5v. Don't feed the nano with 9v, feed it with a regulated 5v direct to the Vcc pin.
I would consider moving the input connector to where U1 is and moving the U1 etc up to next to the SD card. It just seems the major input traces end up at the bottom of the board.Where ever the input connector lands, you need to add 0.1µF from each input pin to ground. You need to have the resulting "cluster" in a very tight layout. You should also have your regulator in the same area, keeping all the "power" components close to each other with a ground plane around it (i.e. the above mentioned ground pour)On your led and button I/O you will need to put capacitors resistors and a zener on each one. If not you will slide across the seat touch a button and the ESD will fry your Nano.Automotive +12V has some nasty characteristics. There are fast high voltage spikes and some lower longer ones. It also runs from 8V starting to 15V (intermittent) charging. Can your regulator handle the power at the higher voltages?
Try not to "push" the manufacturer to their limits on trace widths, gaps, or vias. It's easier to make a board with fat traces with plenty of space-in between. You are less likely to get a defective board, plus you are less likely to create a solder bridge or to damage the board during soldering/assembly/testing. No time to do it right the 1st time, but there's always time to do it over!
Regulating with 5v does make a lot more sense. Take load off of the nano regulator and already have a regulator that's sole purpose is powering the nano. The main reason was that I have a bunch of the 9v regulators on hand, but it would be worth it to buy the 5v versions. Swapping in a 5v regulator would also help clean up a few extraneous traces as well.
Don't get a linear regulator: you have to drop 7V to get from 12V to 5V, that's a lot of heat to deal with!Instead look for buck (step-down) converters, much more efficient, and they can easily deliver 1-2A without breaking a sweat. A linear regulator needs a good heat sink to do the same.
Something more like this: https://www.ebay.com/sch/i.html?_nkw=dc-dc+step+down, https://www.pololu.com/category/131/step-down-voltage-regulators or https://www.digikey.com/products/en/power-supplies-board-mount/dc-dc-converters/922?k=&pkeyword=&sv=0&pv183=6782&sf=0&FV=ffe0039a&quantity=&ColumnSort=0&page=1&pageSize=25Ebay parts are cheaper, but bulkier and of generally cheaper design (you should also derate their max current by about a third). Don't try to design your own DC-DC converter on your first pcb design. DC-DC switching converters are highly layout sensitive.
When you say "highly layout sensitive", what are the consequences of a poor layout? Does voltage become less regulated? Current capacity reduction? Lots of noise?Actually looking at the LM2596 instead of my original post with the LM2678. The LM2596 seems to be the IC of choice for those cheap DC-DC bucks. The datasheet (here) has a "typical application", which looks almost identical to the ebay buck boards. What about just using the PCB layout of the cheap boards, but integrating onto the main PCB?