Adding extra ground traces to keep return paths from switching layers - Page 1
Forum section: electronics / projects

author: amaschas
author_rank: Regular Contributor
timestamp: November 18, 2023, 07:23:46 pm
content: Hey all, I've been working on a 3 channel LED driver board for a while now, and the design process has proved to be very educational with regard to management of signal bleed and noise (as have all of the Robert Feranec). Because the use case requires very high frequency, high resolution PWM control of brightness, there are intrinsically a lot of (relatively) high power lines switching on and off with transition times < 10ns. As a result I've had to think a lot about where those lines are routed and what the return paths for the current are. I've done a lot of work to keep PWM lines, switching nets and anything else that changes rapidly to a single layer, which has had a dramatic effect on the overall noise. Recently I was considering the connector that interfaces the driver board with the LED emitters that it drives, and the fact that the ground pin on the connector reaches ground through a via rather than a trace. I know this is a bit nit-picky, but I'm interested in this more in terms of understanding the way power flows in the board and the effects that it has rather than practically optimizing my board. My sense is that a shorter, more direct ground return path is always going to better, but does it actually make a difference in this case? I've included a image of the board with return traces for ground added (for only two of the drivers, haven't figured out how to route the middle driver), as well as the overall board layout and a schematic for the driver portion. Any feedback would be appreciated!

author: ajb
author_rank: Super Contributor
timestamp: November 18, 2023, 11:03:20 pm
content: Looks like there are three visible layers, is the fourth a solid ground plane?The important thing to remember with return currents is that they are concentrated in the path of leastimpedance. At DC resistance is all that matters, but when you get above audio frequencies inductance dominates. For a track routed above a solid plane, high frequency return currents will follow the path of the track because that minimizes the loop inductance. Even if your PWM frequency were really low, the fast rise and fall times have high frequency components that need to be dealt with.For general signal routing, the best solution is always* to route your high frequency nets over a solid ground plane on an adjacent layer, and to not route over any splits in the plane. A power plane can be substituted for the ground plane with some caveats. If the signals are not ground-referenced, or you can't manage a solid ground plane, parallel return tracks for each signal are generally the next best thing. Either way, you need to be looking at the loop area enclosed by the signal and it's available return paths. The path that encloses the smallest loop area is where your high frequency return currents will go. If you already have a solid ground plane, then you already have the best possible return path for both high frequency (smallest possible loop area) and DC-low frequency (planes are wide, therefore low DCR) return currents.Vias are not as radioactive as you might think when it comes to SI/EMC. Yes, they represent some additional impedance, but if a via allows you to eliminate a big looping path around some obstruction then it's still likely a net benefit. You do need to take care when high frequency signals change layers because the coupling to adjacent planes changes.* Of course there are exceptions, but they are more rare than you might think.

author: amaschas
author_rank: Regular Contributor
timestamp: November 19, 2023, 02:34:14 am
content: Quote from: ajb on November 18, 2023, 11:03:20 pmYes, there is a fourth solid ground plane, thanks for pointing that out, didn't notice I had hidden it! My stackup is Signal - Ground - Power - Signal, and the top signal layer has all of the PWM and switching lines on it, whereas the bottom layer only carries signals that switch slowly or irregularly like the big group of traces at the bottom that route to a separate board with potentiometers and enable/disable signals for the driver. I mostly chose this stackup because it let me put a ground plane under my high frequency signals, and the power plane made it easier to route everything.So if I understand correctly, as long as I'm as I'm routing to a ground plane right under the signal plane, a trace isn't going to make much of a different relative to a via?

author: David Hess
author_rank: Super Contributor
timestamp: November 19, 2023, 04:07:11 am
content: Quote from: amaschas on November 18, 2023, 07:23:46 pmAs pointed out, the impedances determine where the current flows. A ground plane minimizes the impedance for multiple connections making it generally the best solution.I have done two layer boards without a ground plane where I added return current traces between fast and high current nodes, so return currents could take a direct route outside of the power distribution network. This works when you cannot have a ground plane.

author: ajb
author_rank: Super Contributor
timestamp: November 19, 2023, 09:31:04 pm
content: Quote from: amaschas on November 19, 2023, 02:34:14 amGenerally, probably, yes. If the spacing between the return track and the forward track is larger than the spacing between the forward track and the plane, then the track will have a higher inductance because it encloses a larger loop area, and the plane will carry most of the high frequency currents. If the return track has a higher DC resistance than the via+plane, then the via+plane will carry most of the low frequency currents. If the via becomes a limiting factor, you can always use multiples.