There’s no reason that Pin 3 (and also Pin 2, but I deleted all connections to try to fix it) should be part of the GND net, as seen above. I built the circuit using the latest stable OS X build, but when I ran into this issue, I tried downloading the newest version, hoping that would solve the issue. It didn’t, but it did give me the cool “Highlight Net” feature, which illustrates my issue very well.
Why is it part of the GND Net??? It’s only connected to an input on the IC. I had it connected to some other components that were tied to ground, R8. R2 was tied to R8 and GND. The unconnected side of C4 was tied to Pin 2, and the open end of C7 was also going to GND. The NetLabel that is attached to the wire on Pin 3 is labeled “In-_Pin3”, but that doesn’t show up anywhere in the NetList, nor do some of the other labeled Nets…
I tried to attach a snapshot of the NetList that shows this Pin is part of the GND Net, but I’m a new user so I can only post one image. :-/
What am I doing wrong, or what is the software seeing that I’m missing?? Or is there something messed up somewhere?
Please help, I’m tearing my hair out… and I don’t have much to spare up there…
You seem to have very small (fontsize) labels next to your pins (i can’t read them in your screenshot.) are any of them used multiple times? My advice would be to delete all of them and see if there is still a connection.
Are you aware of the fact that invisible power input pins are global labels?
Looking at the picture, the only way you could get this is if C3, C4 and/or C7 have a top pin with name GND. There really is no way that the ned connecting C3, C4 and C7 would be tied to GND, as we can see a complete sub-circuit. If C4 and/or C7 would have a top pin with name GND, this would result in what we see. and if C3 is a copy of C4/C7 then it would also explain the net IN-_PIN3
Rene was correct. There were labels that were used multiple times, on different parts. This whole circuit was built in Eagle and converted over, hoping to minimize the amount of work it would require. In reality, I should’ve just re-drawn the whole thing from scratch in KiCad. Was probably more work trying to fix problems!
Well in eagle a “label” shows the name of the net it is connected to. In kicad a label sets the net.
Just out of curiosity how did you convert your project? If you used the new kicad internal converter this might be something that needs to be addressed.
