In my opinion, it is quite a restriction that shield pins in the symbols are currently combined to one schematic pin.
Do you all connect always both/all shield pins to the same net?
I don’t. Consider a large connector (D-Sub) capacitively coupled to “GND”:
A copper trace between the shield pins will not help reducing the impedance. You can’t beat the D-Sub shell’s low impedance with a thin copper trace.
If you want a really low impedance coupling, you need capacitors on both ends. Again, connecting them on the connector side by an additional copper trace won’t help.
Another scenario: Maybe you want to connect only one shield pin? This would cause a DRC error to be ignored. It would be much cleaner to indicate the NC in the schematic.
I have to admit that changing all shielded connectors now would be rather disruptive (maybe even divisive) since it would affect symbols and footprints.
Nevertheless I wanted to point out the drawbacks of the current state and open a discussion how you deal with it.
Could you provide some example you are talking about?
It depends. Sometimes it is necessary to connect the shield connector to Earth (not GND). Sometimes is it not necessary and you can connect shielding to GND without problems.
I always connect shield pins. As they are connected internally, connecting to different nets is actually shorting them. Leaving some open is reducing the effectiveness to discharge ESD.
You don’t have to connect them to each other with a wire. If they are THT, they will all connect directly to the GND plane on the PCB. for SMT, use via’s to connect each of them to the GND plane individually.
Why would you want to do that?
I don’t like KiCad’s default of pin stacking for power pins. I usually unstack them, so all power pins are visible on the schematic. KiCad is used by many people, and you can’t expect them to all have the same idea’s. So just manage your own libraries for when your own idea’s deviate from the “most common demeanor”.
There are several situations where you must not connect cable shields directly to GND to avoid LF/DC current. So if you don’t want to put a capacitor on each shield contact, you just can let the unused pins open.
As davidsrsb said shield pins are connected internally so you can use only one shield pin for this purpose.
I usually do it this way and discard DRC error for the unconnected pin14 of J5
A variation on this is where the shield is connected to the casing and Signal GND is floated. In this situation I usually place a perimeter zone around the PCB for case ground. Not connecting shields to the enclosure is a good way to fail ESD tests.
in the example I posted, the connector “shield” is attached to the enclosure, and “GND” needs to be coupled capacitively to enclosure/connector to provide a RF path but not a LF/DC path. That’s not really an unusual configuration.
Depends on the project, but yes, I prefer the shield pins to be separate from any other pins and thus the schematic can drive how they are used. Tied to GND, capacitively coupled, left floating.
