When I connect one of the four pads in the PCB, airwires remain on the other pads unnecessarily. I could leave them unconnected and ignore the DRC warnings, but it seems like there should be a way to indicate in the footprint that connecting any one of the pads is electrically sufficient.
I understand that pads with the same name sometimes must all be routed (GND pins for example), but for shield pins, this is often not the case.
Does anyone know if this is currently possible in KiCad, or should I file a feature request?
The pads are named/numbered the same (“SHEILD” using the “Pad Number” field).
The thing is that I don’t want them to be required to be connected together as they are already internally connected by the component since it is a shield. Only one pad needs to be connected, after which the airwires on the other pads should be satisfied.
Here is a screenshot of the footprint, showing they all have the same “Pad Number” which is “SHIELD”
'tis an FAQ. The answer is “not yet”. But it’s in the next version of KiCad! The new feature is called “jumper” footprints, referring to the part itself acting as a jumper between the pins. Check out the links at the bottom of the linked post for further discussion / use cases.
Until then, you’ll have to either:
Diligently connect them all, even though it could be considered redundant.
Ignore the DRC rule.
Modify the footprint so the pads don’t have the same name.
No! You really have to connect them all. If you do not connect them all, you get situations where your gadget does not work with all cables, or the gadget does not work when the cable is plugged in “upside down” or other such things.
And for the shield pins. Connect them all to GND. I didn’t read the whole reference below, but it seems to link to official documentation.
My example does not concern the GND contacts of the connector, but rather the shield legs, which as long as one of them is connected to GND, the others are purely mechanical since the shield is one singular piece of metal.
The official USB-C specification (as mentioned in that thread) does state that “Shield and GND grounds shall be connected within the USB Type-C and USB 2.0 Micro-B plugs on both ends of the cable assembly” and I am not suggesting otherwise. I am connecting Shield and GND through a ferrite.
This is a common technique suggested by a number of application notes. Here’s one from TI in SPRAAR7, see the passage highlighted in blue:
So you add a ferrite bead. In between what nodes are you connecting that ferrite bead?
If the ferrite bead “Prevents EMI from getting onto the cable shield”, then all your EMI stays on your PCB, and it has to be manage by the GND and signal wires, which is very yuck.
I’m not an USB expert, but I do know that there is very stubborn faulty practices “out there”. And that (unfortunately) includes application notes.
My gut tells me you’d want the lowest impedance possible in your GND lead between your USB device and the host (PC). That way, your whole cable assembly and USB device may work as an antenna, but there will be no EMI / signal differences between the plug and your device. And whether RF signals are coupled into this antenna, depends on what the host (PC) does. and those USB port shields are very likely hard grounded over there.
But this is a KiCad forum, and not an electronics design forum, so I’ll leave it at that.
Think of ferrite cylinders that many cables have on them near their ends. They work for all wires including cable shield.
They really help reducing EMI even thinking your way “all your EMI stays on your… device, and…”.
This works like CM choke. If you don’t want to have such big cylinder you can get partially similar effect by inserting ferrite beads in all wires (including shield and GND).
Yes, but OP has a ferrite bead between the shield and the GND on his PCB. The shield will have a lot of capacitive coupling into the cable conductors, and a single ferrite bead in only that location just seems like a bad idea.
Thanks for remark this FAQ for the next version of Kicad. I have several designs with the same dilemma: USB, Ethernet connectors, etc., but especially many SPST touch buttons with four terminals in a single PCB:
In this case, and due to the density of some designs, it is not feasible to connect all terminals redundantly. Ignoring/excluding DRC rules can be very tedious, and I am too lazy to modify footprints that I already think are correct.
These shield joints take a lot of abuse and often fail, so using at least two pads is a wise backup.
Ideally the shield should connect to a metal enclosure. I often used to see a ground ring around the perimeter of a PCB, connected directly to the casing.
A ferrite clamp on the cable itself add common mode inductance to all the conductors, not just the shield and is effective.
