Possible to permantly tie footprint pad to net?

when i use switches, i always connect the mounting pads to ground. i can force this in pcbnew by selecting pad and connecting to the net ground. however, for some reason it looses this assignment and i have had to reconnect them many times. the better way is in footprint editor to connect those pads to the ground net. while that option is present, disappointingly it is grayed out.

what is the best way to ground pins that do not (nor do i want them to) explicitly show up on the schematic? i would ideally like to ground them in the footprint, but if that isn’t possible for some reason at least not have it continuously disconnect when explicitly connected.



This should be done in the symbol/schematic level (make a symbol that includes a pin for the mounting pins mapped to the correct pads and connect that to ground in the schematic)

For inspiration check out the Conn_01x02_MountingPin symbol when combined with the Molex_PicoBlade_53261-0271_1x02-1MP_P1.25mm_Horizontal footprint (we do not have switches like you need but we use the same principle for connectors)

Might be interesting for you: How does KiCad know which symbol pin represents which pad of the footprint?

Thanks Rene. if pcbnew breaks my net connection to that pin for no reason one or two more times i will resort to explicitly putting the ground in the schematic as you suggest.

I will speculate that the connection gets deleted whenever you do a “Update PCB from Schematic” (or “Import Netlist”) . . . and the connection is not explicitly shown on your schematic. Depending on your personality, this behavior is either a charming idiosyncrasy or an annoying quirk of KiCAD. It commonly affects (or is that “afflicts”?) board mounting holes, as well as component pads whose function is mechanical rather than electrical. (Such as, mounting tabs, registration pins, etc.) Searching this Forum should turn up old threads dealing with the topic.

Here are two examples of symbols I have used for tactile switches with mounting pins. They show the mounting pins as “Shield” connections, and the schematic explicitly connects them to circuit common. That way, the connections survive repeated updates from the schematic to the PCB.

User_Switches.lib (1.8 KB)



Dale, that looks like a good solution. Kicad should have a “retain this net list connection through update” checkbox

1 Like

As I remember from discussions here some digital circuits in KiCad library are still defined with hidden power pins. Is’t it what will do the job here. Not visible at schematic but connected in netlist?

I put the mounting pad “symbol” in the schematic like Rene suggests. If it’s electrically connected then it should be in the schematic.


Yes, that was my conclusion too, so I added a mounting / shield to the symbol and footprint

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.