You might want to check (using the full datasheet, not the summary on the LCSC page) that all you unconnected IO pins are in the right states either set to output or to input with an appropriate internal pullup/down. [http://ww1.microchip.com/downloads/en/DeviceDoc/Atmel-7766-8-bit-AVR-ATmega16U4-32U4_Datasheet.pdf](http://ww1.microchip.com/downloads/en/DeviceDoc/Atmel-7766-8-bit-AVR-ATmega16U4-32U4_Datasheet.pdf)<br> <br> I have little exoerience with the ATmega16U4/32U4 and could not find any layout guidelines or reference PCB designs on the Microchip website but: * The routing around the crystal looks poor: The crystal and the 22pF caps need to be as close as possible to the XTAL1 and XTAL2 pins (are you sure that this is running?);  * There should probably be at least a 1uF from VCC to ground plus a 100nF MLCC to ground from every supply pin on U1, especially since you have fed VCC through a somewhere between 0.15R and 0.75R fuse resistance via a horribly meandering and therefore inductive path (Why? Since you have UVCC going to U1 _before_ the fuse, what purpose does a fuse at this point serve?);  * Should there not be a capacitor (1uF to 10uF?) to ground from the /RESET pin to guarantee a power up reset? Please also refer to: [https://easyeda.com/forum/topic/UPDATED-Power-supply-decoupling-and-why-it-matters-30a39d0a77f34d5d8dc77e37c035b3d3](https://easyeda.com/forum/topic/UPDATED-Power-supply-decoupling-and-why-it-matters-30a39d0a77f34d5d8dc77e37c035b3d3)<br> <br>

HI there and thanks so much for your detailed response! Sorry if it seems like I am an idiot or don't know what I am doing as for the most part, I don't haha! This is only my second ever PCB project the first iteration was this board but with holes to physically mount a pro micro, the reason for this one was to reduce the need for assembly and have a USB-C port! This was a pro micro layout I was also looking at but as I say I am still learning so will have more than likely messed something up! [https://easyeda\.com/oshw/Pro\_Micro\_5V\_16MHz\_Open\_hardware\-qJfxrJ1Vd](https://easyeda.com/oshw/Pro_Micro_5V_16MHz_Open_hardware-qJfxrJ1Vd)<br> <br> 1\. Okay so rearrange this to get those components as close as possible\, understood\. 2\. The fuse I added this way as it was how I saw it on the schematic for the pro micro I attached above however like I say\, newbie here\! And I probably completely messed that up\! Can I break a trace to rectify this bypassing of the fuse? 3\. The reset pin on the pro micro in that schematic goes straight to the reset pin on the chip from what I would tell so I added no resistor\! Would any of the above be causing this issue of the device not being detected by windows? I will need to look over the documentation to see if there is anything I need to do for unused pins. Thanks again, Ash

@AKiwi92, 1. poor crystal layout could cause the prrocessor simply to not run;  2. poor decoupling could disrupt the normal operation of the processor;  3. improper power up reset could disrupt the normal operation of the processor.

Yea, that layout is definitely not the best for the solution :D Many things could have been done better if you just rotated some components so the pins are almost pointing to where the other point is supposed to be. Now there are loads of inductors with those vias and anything can happen there. If you have an oscilloscope, you could try to probe the Xtal pins and see if there is a clock there. Check for shorts, double check the schematic, maybe you missed something, I usually do and remember that after I ordered PCB's in the middle of the night :D Also, I don't understand why the USB C connector is on the top layer and everything else is on the bottom, you can easily fit everything on the top. One thing to note was the diodes in the way of the Cherry MX type switches, so I moved them a bit and even in 3D it seems they wont interfere. Another thing is those switches, how are they connected to those pads? Are there SMD type switches like that, do they connect with some springs or solder? I just don't know, I use regular membrane cheap crap keyboards and I'm fine :D The Reset pads seemed a bit weird so I added a 5 cent SMD reset switch with a cap and the pullup resistor. One thing to add maybe would be some ESD protection IC and maybe those 22R series resistors on D+/D- which Atmel recommends in their datasheet. Many nets were moved for better layout and most of the key reading stuff firmware takes care of, so why not. USB can be a cruel mistress, so I prioritized that in the routing. Added more decoupling caps, better placement of the Xtal and its caps. Also, usually the exposed pad should be connected to something, usually GND, but I can't find anything in the datasheet about it and many folks on the interwebz also are boggled about that Atmel had not mentioned anything. Maybe someone who has used an ATMega32u can chip in? While I had a morning online meeting I started to see what could be done better while others are yapping about stuff and came up with something like this during my lunch break :D [https://oshwlab.com/deskpro256/macrokeyboard_fixes](https://oshwlab.com/deskpro256/macrokeyboard_fixes)<br> <br> This may also not be the best PCB design, but I'd say this would work if all connections are fine. Give 10 people to design a board and you'll get 10 different designs :D  <br> <br> 

@deskpro256 Wow! What a comprehensive reply, I totally get what you are saying. Thank you so much for reworking it, it looks amazing! Once thing I think I need to fix is a 10k resistor between HWB and Ground. And you are right I need to add the 22 resistors to D+ and D-, I will give those things a try now and then take a look over everything! The switches use Kailh Hotswap sockets which is what will be soldered to the pads :D also what do you use for getting all the parts in 3d on there? I can neevr figure out how to export that! Thanks Ash

@AKiwi92, "...what do you use for getting all the parts in 3d on there? I can neevr figure out how to export that!" **Tutorial >** [https://docs.easyeda.com/en/PCB/PCB-View/index.html](https://docs.easyeda.com/en/PCB/PCB-View/index.html)<br> <br>

@andyfierman thank you I will take a read! @deskpro256 I have been working on hopefully getting this right and hopefully am at a place where I can order another prototype! [https://oshwlab.com/AKiwi92/macrokeyboard_fixes](https://oshwlab.com/AKiwi92/macrokeyboard_fixes)<br> <br> Just going over the schematic constantly and checking my traces but am some point I’m going to have to bite the bullet!

@AKiwi92, "...going over the schematic constantly and checking my traces but am some point I’m going to have to bite the bullet!" It's not a haphazard path to submitting a PCB for fabrication, it needs some discipline. You first need to ensure that your schematic is complete (no information is missing, BOM info is correct, pinouts are correct, footprints are correctly assigned and pin mappings are correct etc., etc.) and that it is correct (everything is wired up correctly, i.e. the connectivity is correct). The Schematic Design Manager is an essential tool for this. Then you convert that complete and correct schematic to PCB and place everything where it needs to be (and not just where it looks nice). Then route it. Then check the design rules. The PCB Design Manager is an essential tool for this. If you follow the Design Flow in the Tutorial (1) and the two sets of Essential Checklists (4) and (6), in Welcome to EasyEDA (2) in: [https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a](https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a) then you should get to the point where you are confident that your board is good to submit for fabrication.