I’ve resaved and reimported the netlist with various settings. Basically, pin 7 is an hidden pin with a no connect symbol so I don’t even see it in the schematic but it is connected in PCBnew.
I’ve opened both symbols in the editor and they are the same symbol. No duplicates that I can tell.
Just now deleted the connection to R2 and it now show connected to pin 7.
Move R2 and resave and reimport netlist and it is gone.
Move R2 back to original position & repeat, the connection is back, but I notice something odd. The connector circle at the top of the resistor disappears as though it is connected. It only happens in that one spot.
I just did an archive before I remove the resistor and try again. Nope, that spot is ‘poisoned’.
Doh! I’m connecting to a hidden pin. The connection is allowed even though it is marked no connect. It didn’t show up on the other side because the part was mirrored. I’ll post this even though it makes me look a tad foolish because I don’t ever remember seeing that as a reason not to do hidden pins. Or I’ve forgotten.
I suppose one could argue a hidden pin marked NC should never connect?
Yeah. Definitely a mean one. Connecting to non-visible not-connected pins is surely not a good idea, heh.
Cool that the R2 symbol in the last EEschema screenshot even shows as connected to something (circle missing).
Is this a nightly or a stable?
I had the version info but edited it out once I confirmed it was my mistake.
Application: kicad
Version: (2017-10-03 revision 3d1569081)-master, release build
We now try to move nc pins inside the symbol box
(the connection point at the same place as the outlining rectangle.)
But we got this idea only a few months ago so there are not that many symbols in the lib that are built that way.
If someone has a lot of free time, this might be a good beginners project. Maybe it could even be scripted.
I wondered why that was done as it looked messy in the symbol editor. Now I know why and had a quick go though my custom library to try to catch the ones that were not done that way.
I suppose one could argue a hidden pin marked NC should never connect?
I think one could argue that if the schematic editor is going to make a connection to a hidden pin like this, the pin should become visible! But then again, bigger fish to fry etc.
Personally I avoid hidden pins completely, I can’t think of a single valid reason to have hidden pins. I am surprised, and disappointed, that even after the hidden power pin fiasco there are still hidden pins in official library symbols.
Moving the end of hidden pins onto the symbol box line has proved useful, as it helps to prevent erroneous connections (probability to make an unwanted connection is minimized)
