Is there a way to single accept warnings, when footprint pins have no symbol pins?
This is something very common.
I like the check for this warning and would hate to completely silence it. But on the other hand I will get hundreds of them, making me overlook warning which do matter.
Ideally the shown menu would have a knob, with which I could accept a single warning, so that it gets moved from warning list to a accepted warning list.
One way to avoid such warnings is to remove the pad numbers from the unused pads in the footprint.
I’m wondering a bit in which ways KiCad could be improved for situations like this.
Also considering this other recent thread, in which Update PCB from Schematic [F8] “complains” about via’s.
First thought is to show coordinates and/or pan to the location where the error (or warning) is just like DRC. That works for the via, but not for the pads that are not found in the footprints. The ability to suppress certain warnings or warning classes (Similar method to what both ERC and DRC already uses) may work for the issue in this thread.
I also have some such warnings.
Didn’t tried it but what if you add these lacking pins to symbol and hide them.
I remember long time ago (in Protel) I used 100 pin IC that I had lot of its pins to be connected to GND. I have added a vertical column of pins inside IC rectangle (between left and right pin names columns) and connected them to GND (all inside IC rectangle).
If you add such pins, but hidden than KiCad should not have a problem with “no pin…” but may be will have a problem with “no connected” or something like that, but may be it is only in ERC you can not run.
Interesting ideas. Things like this are not so easy to implement all good/safe/easy to understand for all and everyone, but as the thread starter suggest it may be an idea to try to implement a way of silence unwanted warnings, maybe with a RED button or cross 
This so the user understand this might be toxic for the project.
Yep, your idea works!
I simply added for every unused Pad a hidden pin in the symbol.
Works perfect!
A slight improvement to this would be to move those pins inside the symbol outline so that you can’t accidentally connect to them. This is the convention used in the official KiCad library, for example.
Edit: stacking like this also connects the pins, so if you don’t want them connected in the net list, you should set the pin type to unconnected (see Schematic Editor | 8.0 | English | Documentation | KiCad)
You are right. I moved the pins inside.
Also I separated them, since stacked pins will be connected to each other:
In the schematic of cause one has to place “No connect flag” to these hidden pins:
The ERC arrows nicely show the possition of the pins.
Marko
Instead of separating and using no-connect flags, you should be able to leave them stacked and change the pin type from passive to unconnected.
if you do so, then you will get this ERC warning:
The final solution is, to have them non stacked and with pin type “unconnected”.
Thanks - that made the solution perfect!
Marko
