BUG
Concise problem statement:
On the schematic the resistors R9 and R11 not connected to D9 and D11 pads of Nano circuit while on PCB layout them becams connected. I tried to delete the connection of R9 and R11 and the components as well, but once I restore the schematic it became connected again.
![Schematic][1]
![PCB][2]or/20161017/5803d7b6d0ab3.png
[1]: /edit
[2]: /editor/20161017/5803d7db18c6f.png
Thank you.
P.S. Please note I am new in easyeda (actually it is my 1st circuit in this application) and maybe I do something wrong or/and don't provide enough information. I apologize in advance.
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.
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):
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.
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
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.
scroll down....
Thank you Andyfierman for detailed answer. Well done.
I repaired the problem and learned on the way about more easyEDA capabilities.