----------------------[ Testing PCB ground plane myths: ]----------------------- Publication date: 1701474847 This testing was done at low frequency (50 MHz) to replicate the conditions in a typical hobby project. Things will be very different at multiple GHz. I designed a (1.6 mm thick) board with pairs of 15 mm traces and 2 mm of clearance between them. Both for capacitive and inductive coupling, parallel tracks are the worst case. Each end of the traces has a pin, and if a ground plane was present, a ground pin was placed by the trace. [IMG board.png ] One pair has no ground plane, another just a basic one on the back, and the rest have variations on ground planes: - A split ground plane between two traces. - A split ground plane with traces running across the split. - A ground plane with a traces jumping onto the back layer. - A ground plane on both layers - A ground plane on both layers with vias alongside traces. - A ground plane on both layers with a shield trace - A ground plane on both layers with a shield trace and vias alongside traces and on the shield. I ran tests with a 50 MHz sine wave, which is fairly low frequency: The wavelength is much longer then the traces. Capacitive coupling: #################### To measure capacitive coupling, I connected a function generator set to a 5v 50 MHz sine to one end of one trace, and a scope to the other end of the other trace. For tests with a ground plane, I removed the stock ground lead of the scope probe, and used a short (<2cm) length of wire from the probe's ground ring to the ground pane. For the tests without one, I just clipped the scope's ground clip to the function generator's ground lead. [IMG c.png ] The scope probe has ~10 pF of capacitance to ground, around twice that of a 74HC gate input. These measurements are only accurate to around 5%:pay no attention to milivolt differences. Peak-to-peak voltage Configuration 800 mV No ground plane. 340 mV Standard ground plane. 352 mV Split ground between traces. 360 mV Traces over split ground. 351 mV Broken ground plane (across). 340 mV Broken ground plane (along) 294 mV Double sided ground 300 mV Double sided ground + vias 88 mV Double sided ground + shield trace 48 mV Double sided ground + shield trace + vias A ground plane reduced capacitive coupling by more then 2 times. Splitting the ground plane worsened coupling. A double sided ground only improved things if both sides were connected with vias right next to the trace, and worked much better if shield trace was added. At least at this much-smaller-then-a-wavelength scale, a short trace under the ground plane has a fairly small effect. I also measured the signal coupled into the main trace from the one crossing it at 153mV, significant, but not as nearly as bad as a parallel run. Another thing of note about a ground plane is that traces over it have a significant capacitance to ground of around .7 pF per cm for the 1mm wide traces I used. This can cause trouble for high impedance signals, even on relatively short traces. Additionally, this capacitance will only get worse the more layers the board has, especially with the common habit of placing the ground/power planes in the middle layers of the board. The driving impedance matters a lot for capacitive coupling: When the victim trace was driven through a 100 Ω resistor instead of being left open, the coupled signal dropped to ~1/4 of the original voltage. Inductive coupling ################## For inductive coupling, I alse used a 50 MHz sine, but grounded the other ends of the traces. I also added a ~10 Ohm current shut (10mV = 1mA) to measure the current flowing. [IMG l.png ] Again, these measurements are only accurate to around 5%, so pay no attention to single milivolt differences. Shunt voltage (More is better) Coupled voltage (More is worse) Trace configuration 8 mV 62 mV No ground plane 12 mV 26 mV Standard ground plane 11 mV 28 mV Broken ground with trace (across) 10 mV 29 mV Broken ground with trace (along) 8 mV 44 mV Split ground between traces 9 mV 28 mV Traces running over split 11 mV 28 mV Two layer ground 9 mV 22 mV Two layer ground + via stitching 10 mV 33 mV Two layer ground + shield trace 10 mV 7 mV Two layer ground + shield trace + vias The results here are similar to the capacitance results, and don't undermine any of the conclusions made there. While it looks like inductive coupling is insignificant compared to capacitive coupling, it can effect traces with a very low driving impedance. The current I used was just a miliamp, not the several amps common for driving MOSFET gates and the like. Does any of this even matter? ############################# While 50 MHz seems quite high, this type of coupling can easly happen with digital signals. Even of the frequency of a square wave is just a few kilohertz, it can have harmonics up into the hundreds of megahertz depending on the rise time Digital lines themselves are fairly resistant to interference because of the low impedance output and large gap between logic levels. However, most projects at some point deal with analog signals, and these signals can easily be interfered with by fast switching digital lines. The simplest fix is to physically separate digital and sensitive analog sections, as well as avoiding parallel traces between them. Keeping the supply clean with decoupling capacitors, ferries and ground plane is also very important. High impedance lines are problematic, so avoiding them if possible and keeping them short is ideal. A via stitched shield trace over a ground plane is a good last resort. Another statagy if coupling is unavoidable is to simply slow down the digital signals, for example by placing a 5 kOhm resistor in paralel with the output. This won't effect low speed signaling, but will slow down problematic edges. Another case is when the return path for current is not ground, and for that a ground plane is a lot less effective. In this case simply route the PCB so that the signal trace and return path as as close as possible, and keep the overall length short.