I have a schematic with a symbol that has a number of pins. One set of pins I connect to wires with a bus, and it has green dots at each wire-pin connection. But another set of pins I also connect to wires with a bus, and it does not have the green dots at each wire-pin connection. I think it is correct NOT to have the dots. What is going on? See the attached screenshot. Both sets of pins in the symbol are defined as Input pins.
I figured it out. If you look at the symbol in the symbol editor, and zoom in really close, you can see that the pins on the right do not quite meet the shape. There is a tiny gap between, e.g., the left edge of the A30 pin and the vertical line it should be coming from.
Hello and welcome @brandon.arnold
I think you will find a small unfilled green square inside those junction dots. Please delete a junction dot and check.
Did you create your own symbol or is this an imported or Kicad symbol?
Thanks! The green square is indeed there, and yes, this is a custom symbol. As I mentioned in the followup, I found that editing the custom symbol, and getting rid of the tiny gap between the pin and the shape, fixed the issue.
Hi, you didn’t mention editing the symbol. I wasn’t sure how you accomplished this.
The best way to create a symbol is to set your grid to always be 50 mil when you are placing and moving pins during the creation. Only change the grid from 50 mil when you are drawing the graphics.
I was playing:
The junction dots only appear if the wire end and pin end overlap. If they do not quite reach each other only the “unconnected” green square shows.
pin 3 is 4 mil too short, down to pin 7 is 1 mil too short.
10 is OK
1 is 1 mil overlap down to pin 12 is 6 mil overlap.
A bigger picture shows the green “unconnected” square inside the junction.
Just posted this in case anyone was curious. 
1 Like
Failing to do this catches so many people out. KiCad is entirely dependent on exact pin to wire connections on a 50 (arbitrary unit) grid. It seems far too easy for people to change the grid without being aware of the consequences. I would favour a warning banner when any symbol on the schematic has been placed or adjusted such that pins do not sit on the standard grid. Probably needs to be a selectable preference for any individual using custom libraries on a weird grid.
1 Like
Thanks for the great explanation, @jmk and @John_Pateman . Definitely a much more detailed solution. I will keep this in mind.
1 Like
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.