@akles98, Assuming that you have read the Tutorial then sections (2) to (6) in: [https://easyeda\.com/andyfierman/Welcome\_to\_EasyEDA\-31e1288f882e49e582699b8eb7fe9b1f](https://easyeda.com/andyfierman/Welcome_to_EasyEDA-31e1288f882e49e582699b8eb7fe9b1f) should help. I can have a look at your schematic. You can share it publicly:  or privately with me at `my username @ easyeda.com`: 

@andyfierman I've sent you the invitation. Thank you for replying.

@andyfierman I've sent you the invitation. Thank you for replying.

OK, found your shared project but because I can't edit or save an edited copy of your files back into your project as I'm only an observer here are my comments so far: 1. Add 100nF decoupling for U1 3.3V & VCC. 2. U6 pin 18 (AVCC) needs decoupling cap (1uF ceramic?) to ground. Put a 100R resistor in parallel with L1 to damp out possible LC ringing with decoupling cap. Do not fit if ringing is not evident when pin 18 observed using oscilloscope. 3. For clarity extend wires on C4, C5 and U3 pin6 to avoid wiring at right angles directly across the end of symbol pin and to avoid 4 way crossing which could be misread or an accidental join. Best to do more than 3 wire joins as staggered (i.e. max of 3 wires at any one junction). 4. Check other components for wiring at right angles directly to the end of symbol pin. Just makes it easier to read schematic when green net wiring is visible at all pin junction points. See also (4) and (5) in: [https://easyeda\.com/andyfierman/Welcome\_to\_EasyEDA\-31e1288f882e49e582699b8eb7fe9b1f](https://easyeda.com/andyfierman/Welcome_to_EasyEDA-31e1288f882e49e582699b8eb7fe9b1f) Then see (6) in same for essential checks for PCB.

@andyfierman Okay, thank you very much! I've made the changes. Could you check if there's anything else I should correct? My main concern is the conversion between the different voltages (5v and 3.3v). Especially for the UART and SPI voltage conversions. The datasheet of the 4bit voltage level converter that I'm using for converting SPI voltage level says maximum value for pull-up/pull-down resistors is 47k. That value is too high for the reset pin of U6 and so I'm using a 1k resistor. This means I connected the RESET from the header directly to the RESET of U6. Is this correct or do I risk reverse polarity from 5V leaking into 3.3V supply?

For detailed circuit design help, you need to provide a circuit description and links to datasheets for all the active components. Without that it is not possible to make any sensible statements about things like interfaces and level shifting. To interface two chips at different supply voltages you need to make sure that the input and output voltage swings are compatible. This may be achieved by having the higher supply voltage device have an I/O swing that is low enough to be within that of the device on the lower voltage supply. Alternatively this may be achieved by having the low supply voltage device have an output swing that is compatible with the input swing of the device on the higher voltage supply and an input voltage that can tolerate being pulled above the lower supply voltage (or somehow reduce the output swing of the higher voltage device using some form of potential divider). Lastly, use dedicated level shifting devices.

Hello. I've made changes to the schematic. Could you please check it for errors again? My main concern right now is U1 (TXB0104RUTR), with the RESETprog and RESET nets. In the datasheet it says there mustn't be more than 50kOhm resistance on pull-up or pull-down resistors. But I need a strong pull-up resistor on the RESET pin of U6 (Atmega328P-MU). If you know of a simple way to translate the voltage of the RESETprog(5V) to RESET(3.3V) that allows me to have a strong (eg. 1kOhm) pull-up resistor I'd highly appreciate it! Or would the U1 chip keep the reset pin logic 'HIGH', because of the 50kOhm pull-up resistor on RESETprog? I'm really sorry for bothering you so much with this project. I just really want it to work, and I plan to apply with this project for the sponsorship program, to write an article about it. I don't know what repercussions there are if the project ends up not working. I really appreciate all the help you've given me so far! Thank you and have a good day!

Hi akles98, Sorry but you know what your circuit is for and how you expect it to work. Other people do not: it's just a collection of fairly arbitrary components connected up in some way. It is unreasonable to expect other people to do all the figuring out of this and what the components are. As I said above, you need to provide some sort of circuit description to give people a clear idea of what the relevant parts are doing in your circuit. You also need to provide links to datasheets for the relevant parts. Thanks.

@andyfierman I understand that yes. But only a part of the circuit concerns me, specifically how I'm handling the reset 5V (RESETprog) to 3.3V (RESET) voltage level conversion. The conversion is taken care of with U1 and the RESET is connected to the Reset input of U6. If you cannot help it's okay. I'll do the final checks of the schematic and pcb today. What do I need to do before applying for the sponsorship program? Datasheets: U6: [http://ww1.microchip.com/downloads/en/DeviceDoc/ATmega328_P%20AVR%20MCU%20with%20picoPower%20Technology%20Data%20Sheet%2040001984A.pdf](http://ww1.microchip.com/downloads/en/DeviceDoc/ATmega328_P%20AVR%20MCU%20with%20picoPower%20Technology%20Data%20Sheet%2040001984A.pdf) U1:[https://www.google.si/url?sa=t&source=web&rct=j&url=http://www.ti.com/lit/ds/symlink/txb0104.pdf&ved=2ahUKEwjAgLS-3vDZAhXDGuwKHZMVBI4QFjAAegQICBAB&usg=AOvVaw0pukwU7vOTE-k6vEucqvvj](https://www.google.si/url?sa=t&source=web&rct=j&url=http://www.ti.com/lit/ds/symlink/txb0104.pdf&ved=2ahUKEwjAgLS-3vDZAhXDGuwKHZMVBI4QFjAAegQICBAB&usg=AOvVaw0pukwU7vOTE-k6vEucqvvj)#

It's not so much about whether I or anyone else can help you or not as about you giving enough information to ensure that anyone's critique of your circuit - or part of it - is actually worth anything. For example your use of U1 _seems_ OK to convert between the RESETprog and RESET input on pin 29 of U6 but because you have not said anything about how the corresponding PC6/nRESET pin is configured (as described in section 5.2.5 PC6/RESET of the ATmega328/P datasheet and other sections), it is unclear what this pin looks like as far as pin 5 of U1 is concerned. Table 32-2 of the ATmega328/P datasheet descrbes a Reset Pull-up Resistor, Rrst, as being between 30k and 60k but is not clear about whether this is an internal pullup, configurable for the PC6/nRESET pin or is the allowable range of an external resistor. Without your information, how is someone to know this without wading all the way through the ATmega328/P datasheet and other supporting information and without knowledge of how you have configured the device in your application? It is also not clear therefore if you need to configure the OE pin of U1 so that it is held low until the supplies have stabilised as described in sections 3 and 11 of [http://www.ti.com/lit/ds/symlink/txb0104.pdf](http://www.ti.com/lit/ds/symlink/txb0104.pdf) As I say, you know your circuit and it's configuration, programming and application. It is therefore hard to decouple yourself from all that arcane knowledge that you have and put yourself in the shoes of someone who knows nothing about and to then appreciate just how much info that is "just there" for you is completely opaque to an outsider. If you want a quick "yes that looks OK" then yes that looks OK but if you want an answer that you can rely on then you have a responsibility to provide as much supporting information as possible. Please don't take this as criticism. It is just pointing out the reality of what you are _really_ doing when you ask someone else to "have a quick look at my circuit and see if it looks OK". If that seems to need a lot of effort on your part then (a) it is and (b) you have to ask yourself how much are all the hours you have spent in designing your circuit, schematic capture, PCB layout, programming and so on actually worth to you if you end up with another flaky board? One other point: there are a few parts in your schematic that do not yet have BoM information added to them. Don't forget to go through (4) (and again at (5)) and (6) of: [https://easyeda\.com/andyfierman/Welcome\_to\_EasyEDA\-31e1288f882e49e582699b8eb7fe9b1f](https://easyeda.com/andyfierman/Welcome_to_EasyEDA-31e1288f882e49e582699b8eb7fe9b1f) BTW, for comparison purposes, if you want to get an idea of what is involved in a professional design review then have a read through this: [https://docs\.google\.com/document/d/e/2PACX\-1vRhMMBzCZ\_orIFr56QyqYI8HcWsFA00evgh1cQ\_069MJRU2YUJXGWzyX3mMVnxT\-SNz1mydEicu6Bfh/pub](https://docs.google.com/document/d/e/2PACX-1vRhMMBzCZ_orIFr56QyqYI8HcWsFA00evgh1cQ_069MJRU2YUJXGWzyX3mMVnxT-SNz1mydEicu6Bfh/pub)

`What do I need to do before applying for the sponsorship program?` Sounds like a good plan but I think that's a question that Support can best answer

@andyfierman I'm sorry for seeming ignorant, or for making it seem like I don't want to deal with the final checks for my project. I just wanted someone that's way more experienced than I am in electronics or circuit design than I am to check for errors in my design. I appreciate very much all of your tips and the time you put into helping me - you've already taught me a few things. Thank you for being so helpful! I'm wondering if you could help me with my previous project so I could understand what went wrong - it's a lot more straightforward than this one. All of the circuitry works as it should, except for when I solder in the final MCU. When I power it up there are arcs between the power pins, and after a few seconds it starts smoking under the IC at only one the Vcc and GND pins. There were only two errors in the design that I've found - I forgot to connect one Vcc pin and the filter inductor I chose wasn't suitable for that current (also, I didn't put a resistor parallel to it), but even with these two errors fixed (by replacing the inductor with a solder bridge and connecting the Vcc pin through a wire to the Vcc supply) the problem persisted. If you'd like I could send you the link to the project. Again, thank you for being helpful and teaching me things!

First of all go through the two checklists of (4) and (6) in: [https://easyeda\.com/andyfierman/Welcome\_to\_EasyEDA\-31e1288f882e49e582699b8eb7fe9b1f](https://easyeda.com/andyfierman/Welcome_to_EasyEDA-31e1288f882e49e582699b8eb7fe9b1f) If that doesn't help you spot the problem then post back with the link to the public or privately shared project and I'll try to have a look.

@andyfierman I did all the checks again and I couldn't find any errors besides the ones I've already noted myself. I even checked if the schematic symbol pins match with the actual device pinout, and they do. So I don't really know what would cause the power pins of the Atmega64A (U1) to arc. I added you into the project as a Developer. I hope you can spot the problem!

I suspect that the problem is that you have placed the via at the left hand end of the VCC net through pin 21 of U1, too close to the region occupied by the central GND pad of U1.  The ground pad of U1 can be up to 5.6mm square and so extends well beyond the rectangle defined by the central ground pad of the footprint. It can extend very close to the left hand edge of the copper annulus of the via on the VCC net so even with a nominally sized pad on the actual package, even a slight misalignment during assembly of little more than 0.2mm could short the pad to the edge of the via. That said the via should be covered by solder mask but that should not really be relied upon as an insulating layer. It's best to avoid putting vias under devices like this between the pin pads and any central pad. * Try taking the damaged U1 off the board and look for damage to the edge of the ground pad adjacent to the via. I couldn't find the QFN-64_9X9X05P HAND package in the library, so I can't check the dimensions against the datasheet but even so, the dimensions for the central pad on the PCB footprint may be smaller that those of the pad on the physical device to avoid the device floating on a pool of excess solder under the pad and being squeezed out beyond it under the device during assembly so it is difficult to say if the footprint is actually correct. One point: you have no VCC connected to pin 52 of U1. I haven't looked at the current drain of this device but you might find that the current drain through a single trace might be too much (though I'd be surprised if an 0.2mm track would overheat like as you describe. One other idea: There could be some other device that is being enabled by U1 but which is disabled until U1 is fitted that it causing excessive current flow through this VCC net and socausing the overheating. The question then is which device and why does the track get damaged just at the point you describe?

@andyfierman I took the damaged U1 off the board, but all of the traces seem fine and all of them are covered by the soldermask. As far as I'm aware of there's no other circuit being activated when U1 is soldered on. I even tried taking off U2, but the problem still persisted. Strange.

If you have any blank PCBs, try checking the continuity with an Ohmeter to see if any tracks are showing unexpected connections. Also check your original Gerber files i.e. the exact files that you sent off to get the boards made and not any later ones generated after maybe making some minor changes. You can check them using: [https://gerber-viewer.easyeda.com/](https://gerber-viewer.easyeda.com/) or: [http://gerbv.geda-project.org/](http://gerbv.geda-project.org/) If you are using lead-free solder, check for solder whiskers between pads.

@andyfierman I'm using leaded solder, so no problems with solder whiskers. All of the tracks that go to U1 (Atmega64A) are connected correctly; no unexpected connections. I made sure I used the latest version of the PCB; I've made no changes after I've placed the order.

Hmmmmm. A long shot but could you check that: 1) the pin 1 position; 2) the pin order around the package;t 3) he pin spacing on the physical package and on the EasyEDA PCB footprint matches that given in the datasheet for the device?

All of those things seem to check out. Before I got my hot air soldering station I soldered the pcb with my soldering iron, so the connections weren't guaranteed to be good. I soldered a single pcb and the board seemed to function correctly, I even successfully flashed U2 with a program through U1. The program was simply to turn on Vcc at a particular pin. When I measured the voltage, however, I noticed it was only 4.8V or so - I was powering the pcb with a USB connection. The adjacent pins were around 3.6V, and the further away I got the lower the voltage. Except for the one pin I programmed to output Vcc, the others should've been reading as close as possible to 0V. I then flashed U2 again, this time with an empty program. I measured the voltages again and I've noticed they're all between 1 and 2 volts - again, they should be below 0.5V. I then went over the connections again with my soldering iron and the problems started appearing. It's a lot easier to make reliable connections with my new hot air station now, that's why I think the problem appeared straight away when I soldered a second pcb. These are the only things that I noted. It's very strange.