Grounded Copper between Differential Pair Traces - Page 1
Forum section: electronics / general

author: ChanceMcCrance
author_rank: Newbie
timestamp: April 02, 2023, 05:26:27 pm
content: Hi All,I have a question for the folks who fancy design for high-speed digital.Recently I was looking over a layout I saw online and was a bit puzzled by something I saw in the routing of a differential pair. The designer had intended to have a differential impedance of 120 ohm for the pair with each trace owning a 60 ohm single ended impedance. To give you some context, the designer had routed the diff. pair traces on the top layer of the board with an uninterrupted ground plane on the next layer down (inner layer of the board) and there were grounded copper pours on either side of the pair connected to the inner layer ground plane with stitching vias. That seemed normal too me.However, I noticed that there was a grounded copper pour in between the two traces of the diff. pair (on the same layer). This caught me a little off guard as I had never seen it done on a layout and had me asking the following question. If there is a grounded copper pour between the two traces of the differential pair physically separating the two on the same layer, wouldn't that prevent (or limit the ability) of the two traces to couple to one another? It's my understanding that an electromagnetic field will naturally try to couple to the closest piece of conductive material. Is my logic flawed?I was always under the impression that placing anything physically between the traces of a differential pair (aside from dielectric) was something to avoid whenever possible.Thanks,Chance

author: bpiphany
author_rank: Regular Contributor
timestamp: April 02, 2023, 06:34:45 pm
content: Honestly it is out of my league, but I think this video should be of general interest.And why not this article.https://resources.altium.com/p/differential-pairs-without-ground-it-problemMy guess is that it doesn't matter a whole lot as long as the impedance is correct.

author: ChanceMcCrance
author_rank: Newbie
timestamp: April 02, 2023, 10:46:12 pm
content: Thanks bpiphany!I appreciate you getting the conversation started and like that Rick Hartley video you sent.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: April 03, 2023, 12:38:44 am
content: Diff pairs on PCB don't couple to each other very much, with maximum coupling when they're on top of each other in adjacent layers. In that case, the environment seen by one trace is ground plane on one entire side (at whatever the layer-plane distance is), and only most of the other side is the facing trace. So, maybe say 40% of its environment is the neighboring trace, the pair. You need removed ground plane to get higher coupling, which invites common mode issues (that you only want to have to deal with on wired connections where you're saving the cost of a shield, and potential ground loop issues).Coplanar (side by side, same layer), the cross section is edge-on, which isn't quite as bad as it sounds because the effective thickness is more than the foil thickness -- the electric field fringes out a bit between traces. The result is more like 5-10% coupling.Which also means coplanar ground doesn't do much: it only reduces Zo by say 5%. It's more important for reducing coupling between traces. Which, is an odd choice here when the signals are complementary, but is handy when sensitive signals are present.So, diff pairs aren't being used onboard because they're differential: they're primarily not; they're being used because it keeps common mode synchronized between the two traces. That is, they're exposed to identical environments, at the same time (position along the trace). And this works as long as CMR is respected, which should be easy enough: you'd need a terribly nasty board to violate even 1V of CMR.Tim

author: Smokey
author_rank: Super Contributor
timestamp: December 04, 2023, 04:11:56 am
content: Just watched one of Rick's other videos. He showed this slide:It's actually this board:https://www.nxp.com/docs/en/user-guide/KT33812ECUUG.pdfSmall Engine Reference Design User ManualFeaturing the MC33812 and MC9S12P128KIT33812ECUEVME Evaluation BoardGuess they needed a "REV1"