I have a USB-B connector with two of its TH pins connected to the connector’s shield. Accordingly I have two TH pads on its footprint with the same Pad number (while the schematic symbol has a single pin with its Pin number matching the two pad’s Pad number). I would expect these pads to be connected always on the board in Pcbnew, but they are unconnected by default as shown by the rastnest and the DRC and I need to connect them explicitly with a track.
If I press Rebuild Board Connectivity in Tools/Netlist then the two pads become connected (even without an explicit track between them) but after redrawing the screen with F3 they become again unconnected.
One workaround I found is to delete the Net name from the pad that isn’t connected (explicitly) to anything. In this case the two pads stay connected permanently, until I do a Read netlist, at which point their _Net name_s get populated (since they are connected to other components too) and they become unconnected again.
Is this a bug, or am I doing things incorrectly? Is there any problem by deleting the netname as I described?
I read that something similar can be achieved by overlapping invisible pins on the schematic symbol, but I’d think that’s for the case when the pins have different _Pin number_s.
Following are screenshots about the relevant part in Eeschema and Pcbnew.
I’d say the problem is ‘sorta’ the footprint. In reality isn’t the shield all one piece with two projections? Is it your intention to connect it as shown above with nothing else? That second pad would be soldered to just a through hole to no where? I don’t know if you can remove a pad number. I’ve never tried it but that might do what you want?
KiCad does not understand two pins having an internal connection. In this case connecting both pads is sensible as connector shield pins are prone to dry joints
Yep, I agree now, I could solve this by changing the footprint (and the schematic symbol in my case as suggested by a few comments in the post linked by @Rene_Poschl).
In reality isn’t the shield all one piece with two projections?
Yes, the shield is one metal piece connected to two “wing” pins (the bottom plate being plastic):
Is it your intention to connect it as shown above with nothing else?
Yes, one of the wing pin would connect to nothing else. The other one connects to other components as shown in my schema/layout.
That second pad would be soldered to just a through hole to no where?
Yes.
I don’t know if you can remove a pad number. I’ve never tried it but that might do what you want?
That is removing the pad number in the footprint editor from the footprint. Yes, that worked too. In the end I decided to make the pin/connection configuration explicit in the schematic as well, so I created a custom symbol with a new pin having its unique pin number and a custom footprint with the unconnected pad assigned a pad number matching this unique pin number (6 in my case). On the schematic I have a “No connect” marker on the unconnected pin. I’m not sure if this is always the best approach, maybe in some cases this would clutter the schematic too much.
Thanks read through it. I use now a custom symbol/footprint with the unconnected pin added on the symbol and explicitly marked as not connected on the schematic, that solved it.
In this case connecting both pads is sensible as connector shield pins are prone to dry joints
Could you explain this? I solder both pins to their pads of course, but I don’t see why connecting them with a trace would help (if that’s what you meant).
In this case connecting both pads is sensible as connector shield pins are prone to dry joints
Could you explain this? I solder both pins to their pads of course, but I don’t see why connecting them with a trace would help (if that’s what you meant).
Ah got it, after a coffee. So that the RC components are still connected to the shield when the joint at pin 5 fails. This sounds sensible, I will reconsider connecting the shield pins after all Thanks.
Thanks.