![Schematic][1] [1]: /editor/20161017/5803d7b6d0ab3.png

Hi Boris-K, Welcome to EasyEDA. Please note that when asking for help in EasyEDA it is much easier for people to offer advice if you lost the link to your public circuit: https://easyeda.com/Boris-k/StabTest-3dd2d96783634ce79ebc950b76d7124f instead of just images. However, having looked at your public circuit, the cause of the problem is that the ARDUINO NANO symbol has incorrect pin numbering. If you click on the symbol and then press the `I` key you will see that several of the pins have been assigned duplicate numbering. This symbol is a user contributed symbol and appears to have not been carefully checked by the contributor. * This is why we urge users to check symbols and footprints very carefully. However, this error is easy to fix. The same `I` Hotkey allows you to reassign the package (PCB) pin numbers on the schematic symbol so you can correct them to whatever they should be (sorry I don't know what that is because there is not link to a datasheet in the Description for this symbol or for the associated footprint. To make this a permanent fix, if you find the part in the SHIFT+F component search again (it is the first entry): ![enter image description here][1] then click on the `Edit` button you can edit the symbol, add the missing Description (with links to suppliers, supplier part numbers, manufacturer and the all important manufacturer's datasheet shwing the pinout and the PCB footprint) and then save it with a new name (to distinguish it from all the other user symbols). Then you can replace the symbol in your schematic with your new, fixed, one. * Please note that it seems that you are attempting to create a PCB from an incomplete schematic: https://easyeda.com/editor#id=5450fa59b05341feaae139a99f31eedf Before trying to pass a schematic into PCB layout, it is important that all parts are present in the schematic, that they are wired up correctly and that they have the correct packages associated with them. This post gives some guidance: https://easyeda.com/forum/topic/The_best_way_to_design_a_PCB_in_EasyEDA-ThR3pwqIC [1]: /editor/20161017/580400877e96e.png

I think if you change pin A4 to from PCB pin 12 to 23 and pin A5 from PCB pin 14 to pin 24, that should fix it. ![enter image description here][1] scroll down.... ![enter image description here][2] [1]: /editor/20161017/58040368d412d.png [2]: /editor/20161017/580403bf42cf7.png

Thank you Andyfierman for detailed answer. Well done. I repaired the problem and learned on the way about more easyEDA capabilities.