I am designing a footprint for a PCB edge connector. The datasheet shows in DETAIL 'A', some "nipples" at the end of each finger. I don't understand note 5 and I don't understand what these "nipples" are for.
From another source, I can see that edge connectors usually have these outgrowth tracks at the edges. What are they? Should I add them to my footprint?
For reference here is my current footprint for the mating MECF-20-01-L-DV-WT-K-TR connector.
Those traces are used to short all the terminals together before the card is cut out of the panel. While immersion gold doesn't require it, hard gold that's capable of surviving dozens to hundreds of insertion cycles needs to be electroplated, and that means all the plated portions need to be electrically connected to become one of the electrodes in the plating process.
The connections are required to short together the fingers so they can be electroplated with thick hard gold (typically after a nickel barrier layer). The shorted fingers become the cathode in the electroplating process. The shorting is removed later in the processing of the bare PCB when excess material is removed and the bevel is machined.
Point 5 suggests making them the width of the finger, the diagram shows something else, but it is X'd out (i.e. don't do this). Not X'ing out the detail view might be a bit confusing, but we are supposed to assume inheritance. They want you to extend the full width of the finger off the final board outline.
If you leave it to the PCB fab you lose control over what happens. Here is what PCBWay considers ideal from their pov.
