Why is UVCC is connected through a fuse to VCC?  If the outputs from the ATMEGA32U4-MU are supplied from VCC then your LEDs are either the wrong polarity or connected to the wrong supply rail:  You have at least one location wheree you have tracks on b oth layers wioth no via to connect them together:  You must check the Design Manager:  Don't just do Convert to PCB and then place parts and start routing. Place the parts that have to go in certain places first then move and rotate the rest around to minimise the ratline crossovers and simplify the routing flow before you start pushing copper. It is worth spending longer in the placement and rotation stages because it saves so much time when you actually come to doing the routing. Route the signal traces first then try to use ground and VCC copper planes to connect the supply pins and decoupling (ground on the component side, VCC on the other side because most component pins will survive a short to ground better than a short to VCC while probing about during debugging). Do you need mounting holes? Please read: [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)

Hi! Cheers on having an idea and trying to make it, as well as asking for reviews of what you have done! :) You have a good idea to sleep on it, that lets you rest and have a clean look at your design later. While you're at it, look through andy's go-to post: [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) Have you got an enclosure for this device or you're going to design it around the PCB? Don't forget mounting holes or don't have components where there are going to be clips for the enclosure. Also, the "max input" for the 5V regulator seems to be 12V(with -20 and +20 being the absolute max): [https://datasheet\.lcsc\.com/szlcsc/1806090830\_Microchip\-Tech\-MIC5219\-5\-0YM5\-TR\_C144182\.pdf](https://datasheet.lcsc.com/szlcsc/1806090830_Microchip-Tech-MIC5219-5-0YM5-TR_C144182.pdf) The device will work when it's got the USB cable, right? Do you need the "RAW" pin at all or is that there because the Pro Micro has it there? What will provide the RAW pin with power? USB-C would still be running at 5V, what other voltages or inputs will this be using? Also, you have the trace that bypasses the regulator, so do you need it or no? Maybe have a SOT-223 package 3.3V regulator if you even need one.  I haven't used USB-C, but I don't think that tying the D1+ and D2+ / D1- and D2- pins together is how you should be doing the data pins. Just use the D1+/- and ingore the SS D+/- pins, the ATMEGA32U4 only has 1 USB port and I don't think this will be a high transfer speed device.  Also, the way you have routed the data lines is a NO-NO. USB is differential, so you NEED to route them next to each other and don't make them so long. This is a USB device, so make that a priority, make sure the USB lines are short and have the connector close to the microcontroller or bad things can happen. Look at some USB routing notes. Also maybe have some data line protection with USB TVS diodes. Another thing is the passive components. Do you really need the capacitors and resistors have 3 different package sizes? You have some 1206, some 0805 and 0603's. I'd suggest choose one and stick to it. For my own projects I usually use 0805(for home etched boards) or 0603 (for ordered PCB's). Just because JLC can solder 0402's doesn't mean you need to use them. Think about servicing this thing if you need to rework something on the board, will you be able to solder/desolder the components? The LED2 and LED3 won't work because their cathode is connected to VCC. Please change that to GND to have a light show. Also, adding to the enclosure, do you want to see these LED's on the outside or are they just for debugging and won't be visible when closed up?  Also, the component names are a bit scattered, you have 1 fuse, but its name is F2, what happened to F1? :) Thanks to the always working developers, you can now easily use the Re-annotate tool to name the components C1,C2,C3 instead of having them C1, C3, C69 etc. Some PCB connections won't work, because you don't have vias connecting them from the top layer to the bottom.  Route your signals first, then your VCC and only then take the Copper area tool and make ground(GND) planes on both layers which will connect all the GND connections together. The ones who don't connect, use vias to stitch them together. Also try rotating the 32u4 45 degrees and move it closer to the USB port, maybe that'll help with easier routing. If the SW1-5 places are final, lock them so you don't move them by accident :) Move the diodes D1-D5, D8 to the bottom layer as that is the layer JLC will solder. You can't have the assembly on both layers, only one. I tried my proposed changes so you can take a look and maybe have some ideas on how to continue your project. This isn't pretty or close being done, just slapped something together in 10 minutes.  But you can see that if you put the 32u4 somewhere in the middle, the rotary encoder is easy to connect and the USB lines route better. Here is how this looks with a GND plane:  I hope all this helps you and your project to become a reality. And as Dave Jones would say, "I hope it fails, so you learn from your mistakes and debugging!" :) Cheers!

Hi both and thank you so much for your in depth replies, you have no idea how much I appreciate it! 1\. I do have an enclosure that I am having made from CNC aluminium\, and I do need to add mounting holes\! I had them initially but started fresh and forgot to re add them so thanks for the reminder :\) 3\. The 5V regulator sub\-assembly was based off of this schematic for a pro micro\, I will be using 5v\, looking at it now does that not mean I can get rid of all of these components and just have F2 going straight to VCC? Does this also solve my RAW issue in that I don't need to use it at all? [https://cdn\.sparkfun\.com/datasheets/Dev/Arduino/Boards/Pro\_Micro\_v13b\.pdf](https://cdn.sparkfun.com/datasheets/Dev/Arduino/Boards/Pro_Micro_v13b.pdf) 4\. As for USB\-C I am connecting A7 and B7 together for D\- and A6 and B6 together for D\+ for the female connection which I think is correct \(female and male pin\-out below\)\, this is only because for the male connection it only uses A6 and A7\, so if plugged in one way I wouldn't have a connection to the B6\,B7 side of the female? I may be completely wrong here so let me know if I am being stupid\!   5\. Great point on the naming and annotation I will for sure clean that up :\) 6\. Vias\, got it\. Didn't know if they were magically added by the software\, wishful thinking and now I know\! 7\. How you got all of that to fit nicely like that is nothing short of amazing I have been wrestling with it all day\! Thank you :\) Do you have a link to the project so I can play around with what you did? 8\. LED's I think I just got them the wrong orientation as the Pro Micro schematic I was using has them going to VCC but the other way\, doh\! Thank you again guys, it was a massive step in the right direction and I have learned a lot, now back to working on it! One thing I did notice which was frustrating was that the AtMEGA I placed, said in stock in the software but not when I go to checkout, so is left out, same with the crystal. Is there another part I could use instead for these which is available? Also another thought, I did eventually want to add SMD RGB LEDs to the top of this board so the user can program keycap lighting in QMK.. but I can't get those soldered on there for me so guess I will look at doing those manually! Thanks! Ash

"...and I do need to add mounting holes! ..." Put them in the schematic. See (2.2) in (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) "Vias, got it. Didn't know if they were magically added by the software..." See: [https://docs.easyeda.com/en/PCB/PCB-Tools/index.html#Via](https://docs.easyeda.com/en/PCB/PCB-Tools/index.html#Via) and: [https://docs.easyeda.com/en/PCB/Route/index.html#Route-Tracks](https://docs.easyeda.com/en/PCB/Route/index.html#Route-Tracks) "I did eventually want to add SMD RGB LEDs ... but I can't get those soldered on there for me ..." Is that because JLCPCB only do single sided SMD PCB Assembly? Have you asked JLCPCB if they can do double sided assembly? What about reverse mounted LEDs and small holes in the PCB? [https://datasheet.lcsc.com/szlcsc/Everlight-Elec-65-21-BHC-AP2R1EZ-3AA_C264593.pdf](https://datasheet.lcsc.com/szlcsc/Everlight-Elec-65-21-BHC-AP2R1EZ-3AA_C264593.pdf) [https://datasheet\.lcsc\.com/szlcsc/1912111437\_MEIHUA\-MHT151WDT\_C401114\.pdf](https://datasheet.lcsc.com/szlcsc/1912111437_MEIHUA-MHT151WDT_C401114.pdf) [https://uk.farnell.com/c/optoelectronics-displays/led-products?led-mounting=smd-reverse-mount](https://uk.farnell.com/c/optoelectronics-displays/led-products?led-mounting=smd-reverse-mount) [https://hackaday.com/2019/04/17/the-science-of-reverse-mounted-leds/](https://hackaday.com/2019/04/17/the-science-of-reverse-mounted-leds/)

Hi there, I'm a beginner at this EasyEda pcb program and to be honest i feel quite old for this, but as it is said, "it's a dirty job but somebody has to do it"..... So, i have already made my first schematic and when i run simulation i get the following message: Fatal Error: Unknown subcircuit called in: XU2 C1\_2 XSC1\_1 U2\_3 U2\_4 U2\_5 U2\_6 GND U2\_8 U2\_9 U2\_10 U2\_11 U2\_12 U2\_13 VCC NO\. Does anybody in here knows what the above sentence mean? It doesn't recognize U2, since is one 74HC14 SCHMITT which exist in spice library. Have i done a connection wrong? Is it something else? Any help will be appreciated. Try in simple English since as i mention above i'm a beginner in this program. Thank you in advance for your quick reply - support. Best regards, Bill.

@bjr1, It looks like you have posted here by mistake. Please read the Forum topic marked as [Must read]: [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) \- in particular \(3\)\, the Simulation Tutorial that is linked to from \(2\) in the above document and is itself marked as essential reading prior to attempting a simulation\. Then, post your question in an appropriate category, clearly and with sufficient supporting information to allow us to help you.

@andyfierman thanks for the documentation! @bjr1 - You will be better off posting your own topic and linking to your schematic :) I have had another go, removed the power regulator circuit, is this safe to do? This keypad is designed to run from 5v USB power at all times. Hopefully my project will have updated in the original link to my new version! :) I am getting 3 errors before exporting gerber but am unsure of where the error is after checking connections. Let me know if there is anything that is glaringly obvious! Yes unfortunately they only offer one side SMD, I can add the LEDs after though if needed and can work this in once this prototype is ready for manufacture! Thanks again, Ash

Hi again, great work! 1\. With a metal enclosure maybe think about having a GND connection to the PCB with a wire link screwed to the enclosure\.  3\. Yes\, if thats the only supply\, the regulator is not needed\, but maybe add back in that 10uF tantalum capacitor or an electrolytic capacitor for bulk decoupling\. You don't need exactly 10uF\, even 4\.7uF or 1uF would do fine\, you aren't making a high power device\. You sgould also have local decupling caps next to your micro for the small surges\, but the bulk capacitor will smooth out the big ripples\. She'll be alright\!  The RAW is unnecessary here, yes, that was only there because on the Pro Micro, you could solder, lets say, a 12V wire to power it. You are powering it from the USB cable, so its not needed. 4\. Yes\, that does make sense\! Carry on then\! 5\. Also try to take care of the silk screen too\, the component designators shouldn't cross pins and should be visible for your own sanity and servicing\!   7\. The more you do it\, the better you'll be at it\. It's like a puzzle\. I've had projects where I redo the board 5 times just to make it fit or route better\. Unfortunately I didn't save it, but I saw that you have most of it done similar anyway, I usually open them up and play around for the help post and then close it :D For the RGB LED's, you could solder them yourself on the top layer, but check the fit with the CherryMX, maybe have that for the REV 2? You'll probably have some more ideas after you get your first prototypes done and feel how easy/hard it is to use. For the schematic DRC warnings, you have labelled pins as the Pro Micro had, but aren't using some of them, you can ignore the warnings, or add the N.C.(no connect) flag to those pins as you have done for pins 40 and 41. Another thing I noticed is that your reference schematic has a different ATMega32u4 symbol. That is, yours has the exposed pad(EP, pin 45) as a pin there. Connect that to GND and a lot of ground connections will be much easier. For the PCB DRC errors, there are a few unfinished things: [x] GND [x] ROW0 [x] SW3_1 These are easy to fix: Again you have the traces going to the component, but not on the right layer :) Some tricks you can use for easy GND connecting [ [Short video showing the issues](https://youtu.be/gJG59SQbtyg) ] Also take a look at your SW2 and the rotary encoder, you have put them on the bottom layer somehow! Set them to the top layer and redo the connections! Also, add a logo/designer text on the silk screen, be proud of your work!   Anyway, you probably get the idea! Have fun!

@[deskpro256](https://easyeda.com/deskpro256) Thank you so much again for your in depth response I really do appreciate it! I now have this design done and am just weighing up costs as it looks like JLCPCB are not great for stock at the moment :( I may put in a order for a schematic that just integrates a pro micro as before as a stop gap! [https://easyeda\.com/editor\#id=\|91d42dde74d34760908782a10bee6310\|1277e2f1b1e34d2eb1e3e9dc6532477a](https://easyeda.com/editor#id=|91d42dde74d34760908782a10bee6310|1277e2f1b1e34d2eb1e3e9dc6532477a) Here is where I am at, much simpler and after all the advice you gave it came together much quicker! Any blatant issues I will run into? I also have a PCB in there for the mounting plate for the switches, which has a bit of subtle branding on! The issue I am having is that this top mounting plate needs to attach to the casing, but I can't have holes in all 4 corners because the pro micro will be beneath it in the top right :/ something to ponder! Cheers, Ash

Apologies, wrong link! [https://easyeda.com/AKiwi92/macro-pcb](https://easyeda.com/AKiwi92/macro-pcb)

Hello, yes that will also work and you can have most the software done on this and later design a full custom PCB when you're ready! For the PCB to PCB connection you could use PCB standoffs. Look up: PCB Standoffs, plastic or metal  snap in PCB standoffs  That should give you some ideas for how you can mount them. Also your PCB looks alright, it has the connections you need and it'll work fine. :) Although I'll do some nit picking that'll help you out in the long run:  Between SW5 and SW6, you have the ROW1 traces going loooong way over and around, keep it simple, your bottom layer has nothing there, so route the trace on the back and it looks neater! I would have still worked, but it just looks nicer :) A lot of older logic IC boards were laid out similarly, by having one layer only have the traces going horizontally and the other layer have the traces going vertically. Just something to note!

@deskpro256 Thank you so much for the help yet again! I have been working on this and I THINK I am ready to place my order. Would you mind giving it a once over and making sure I am not missing anything obvious? Two changes are I am moving the pro micro to the top layer, and having another cut plain pcb on top which will snap into the switches and all be held together with standoffs. The pro micro will sit between those layers soldered to the bottom. Example below: [https://imgur.com/a/BvzcnEp](https://imgur.com/a/BvzcnEp) So I have added pads to the top and bottom layers of the PCB where the mounting holes are so the standoffs don't short anything, from my calculations the standoffs should be 3.3mm wide so I did a 5mm pad to make sure. The top plate obviously doesn't need pads as it doesn't have components! Let me know what you think and thanks again!

Hi, electrically it seems ok. But there are some things you should improve! You seem to have pads for grounding the stand-offs to the PCB, but they are on the top layer, but your GND plane is on the bottom. Also those pads are without a net name. Make their net GND and also set them to Multi layer, as well as remove the holes on top of them as they are creating design rule errors. Having them be on multi-layer, you'll get a hole too, set the hole diameter to your preferred size(2.4mm I suppose) and remove the holes. Plus add a GND plane to the top layer too. That will make the GND connections better.    Also the PCB holes for the switches and encoder should be made with board cut-outs, instead of the board outline tool. JLC might not create the hole as you might think, even if the 3D viewer shows a hole there. Simply take the "solid region" tool and create the same shape over the current board outline shape and then delete the board outline. Set the newly created shape to a board cut-out and set it to multi-layer as well, just to be sure.   This should get you the desired results. Hope this helps you and be sure to check with JLC if what you have make is what you wanted to make, and that JLC will create what you wanted! :)

As I referred to above, putting symbols for holes onto the schematic and creating and assigning PCB Footprint for a dedicated hole and surrounding pad size is a nice touch as it means you can't forget to add them and what they are connected to (or not) is clearly shown in the schematic. There are a few Footprints like that already in the library but they are easy enough to make up. After querying this with JLCPCB, the use of Board Outline and Solid Region set to Cutout seems to be completely interchangeable. :)

Thanks so much guys, really appreciate it! The hole/pad combo I used was just for the standoffs they aren't actually supposed to connect to anything but I will definitely have a look at both of your suggestions now and get a final version ready for JLCPCB :D