Differential Impedance - Page 1
Forum section: electronics / beginners

author: jmsigler
author_rank: Regular Contributor
timestamp: January 31, 2017, 09:06:34 pm
content: Heres a pretty simple question, but I couldnt find a direct answer. Is differential impedance between two signals simply 2x each individual signal's impedance to ground? For example, if I was routing 100ohm differential lvds traces, I would make each signal 50ohms to ground and then route them close enough to couple?

author: jmsigler
author_rank: Regular Contributor
timestamp: January 31, 2017, 09:11:29 pm
content: Ended up answering my own question I think. My understanding is that it is close, but the coupling/proximity between the traces causes increase/decrease on top of the individual single ended impedance?

author: Benta
author_rank: Super Contributor
timestamp: January 31, 2017, 09:39:50 pm
content: Search the web for: HB205/D "MECL System Design Handbook" (you can download it free as pdf)It has a couple of excellent chapters on transmission lines and termination.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 31, 2017, 10:15:45 pm
content: If they are independent, then yes, precisely!If they are close together, then there is some impedance that exists between them, which is comparable to, and acts in parallel with, that normal mode impedance.Or actually, more generally -- when traces are far apart, the impedance between them (excluding the normal impedance through ground) is simply really high. So high that it's negligible in parallel with the normal impedance, so you don't care.Regarding PCB design, I like to say differential routing is a lie -- even for traces only a (minimum clearance distance) apart, the coupling is only about a third the total. So it's still dominant normal mode.This varies with geometry, obviously. A board with pretty thick dielectric layers, and loose tolerances (a conventional 2 or 4 layer proto board build), will have characteristics as above.At 6+ layers, you have the opportunity to try broadside traces (i.e., P and N routed in identical positions, on adjacent layers), which has good coupling.At 10+ layers, with <= 1.6mm total thickness, the dielectric may be getting so thin that you have no choice but to pay for tighter tolerances (4 mil width/space, or even finer), otherwise the trace impedances will be too low.The takeaway lesson is this: even if the differential coupling is dominant, the common mode impedance and voltage will always be there, and can't simply be ignored forever. Most differential interfaces take care of it okay, even if it's a poorly documented aspect (e.g., LVDS drivers have a controlled CM impedance, usually around 400 ohms -- much higher than Z_cm in most cases, but at least it's /a/ source of CM damping). Willfully ignoring it can lead to pulling of hair and gnashing of teeth...(Example: USB. When is differential not differential? USB is a particularly annoying example, because the J/K states are unbalanced. Their mere existence, even though used sparingly (at the start and end of frames), prevents the application of useful CM filtering. This is why Full Speed and High Speed USB is only possible within shielded cables.)Tim