Using guard traces for return current instead of ground plane - Page 1
Forum section: electronics / projects

author: c64
author_rank: Frequent Contributor
timestamp: September 22, 2021, 06:18:03 am
content: Suppose you have two layer PCB with no ground plane. But you can have guard traces (ground traces running parallel to signal traces) connected to solid ground pour on the same layer. Are they good alternative to ground plane?All signals are digital

author: c64
author_rank: Frequent Contributor
timestamp: September 22, 2021, 06:23:41 am
content: Actually, even if you have ground plane on the bottom layer, is it a good idea to have guard traces on the top level as well? They are much closer then ground plane. For typical two layer board it's 5mil vs 1.6mm, more than 10 times

author: c64
author_rank: Frequent Contributor
timestamp: September 22, 2021, 06:34:36 am
content: Here is example

author: capt bullshot
author_rank: Super Contributor
timestamp: September 22, 2021, 07:53:13 am
content: Quote from: c64 on September 22, 2021, 06:34:36 amNothing wrong with that. Back in the days this technique was used to lower mutual inductance coupling on flat wire cables: Every second conductor tied to ground.Distance to nearby GND conductors has influence on the characteristic impedance of these traces, so if you're doing high frequency (>100MHz or longer controlled impedance traces) stuff, you might want to check that. At first glance, doing so (checking the characteristic impedance) appears overkill in your layout example as the traces appear to be short.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 22, 2021, 03:25:18 pm
content: Just how fast are you switching, that signal quality is a concern?Note that the impedance of that arrangement is ~120 ohms, much higher than with a solid plane, and it has considerable common mode coupling, particularly for traces in the middle -- that is, crosstalk between adjacent pairs, as well as coupling to free space (radiated emissions). The best solution for which, is a shield over the affected area; in other words...a ground plane.Also note that minimum distance isn't the important factor: it's the width divided by distance. The width and distance aren't exactly trivial to calculate in either case, due to fringing fields, but the outcome is that edge-coupled traces have much higher impedance, even for minimal separation (say 4-7 mils for typical proto fab), than for a much higher distance above ground plane in a 2-layer build (~60 mils board thickness). Similarly, the coupling between adjacent traces in a bus, over ground plane, isn't as bad as you might think (on the order of 20%), even though the traces are seemingly closer to each other than to ground.And obviously this all improves greatly on multilayer builds (where ground might be 5 or 10 mils away).Tim

author: c64
author_rank: Frequent Contributor
timestamp: September 24, 2021, 03:45:50 am
content: Quote from: T3sl4co1l on September 22, 2021, 03:25:18 pmThis is more like a general question.I have quite a few double side PCBs, traces are usually 6mil, with spacing > 12.5mil. After ground pour most of the space between traces becomes guard traces.Clock frequencies 100-150 MHz or so, rise times 1-2 ns. Never had issues with signal integrity so far.

author: Berni
author_rank: Super Contributor
timestamp: September 24, 2021, 05:17:50 am
content: Guard traces are something different. They tend to be exposed copper tracks around sensitive high impedance parts of a circuit and are often actually driven to a certain voltage rather than ground. The point of them being is to bring the surrounding area to a potential that will cause current minimal leakage, we are talking nanoAmps here.What you have here is instead a ground pour or ground fill. It is indeed a very common way to do ground planes on 2 layer boards. Often coupled with vias peppered all around it to stitch the ground plane on both sides of the board into one big solid ground plane. That way even if a trace is in the way of the return current the current can still zig zag to the other side of the board and keep going.Surrounding traces in ground fill like this is also a valid way of doing it, since any uninterrupted near by ground can serve as a high frequency return path.But as others have mentioned above once you get to high enough speed its all a matter of the trace AC impedance. The track size and spacing will determine how many Ohms of impedance the trace has. This impedance has to match the impedance of whatever is driving the signal and match whatever is receiving the signal. If you don't then signal reflections happen that distort the signal. However this only really becomes significant once the trace is a significant fraction of the signals wavelength. For 100MHz this is 3 meters, since signals in copper coax are slower this is more like 4 or 5 meters. So about 1/8 of that is 50cm (but yes there are higher harmonics too). Most PCBs are not as big as this, so this is why you still get great signal integrity by just simply putting ground close by. However once you get into RF and high speed serial lines that go >1GHz this becomes very important on the distances of a typical PCB.

author: Terry Bites
author_rank: Super Contributor
timestamp: September 24, 2021, 04:55:15 pm
content: All signals are analog!