I am laying out a 10/100Mbps Ethernet PCB with discrete magnetics. From the magnetics to the PHY chip I have a system ground plane on the adjacent layer for the return path. From the connector to the magnetics, I have a plane that is connected to the Bob Smith resistors underneath the pairs, this plane is connected to the chassis ground via 1nF, 2kV capacitor.

My questions are:

  1. should I also connect the system ground to the chassis ground through a 1nF, 2kV capacitor?
  2. I have read a couple of application notes that advise the keep the system ground far away from the chassis ground. How about between system ground and magnetics ground, and between magnetics ground and chassis ground?

PCB capture enter image description here

Top layer: differential pairs + chassis ground connected to one of the mounting screws TOP LAYER

MID-1: Magnetics ground under differential pairs, chassis ground mostly, system ground going to the LED. Distance from system ground to chassis ground is 100mil, and from magnetics ground to chassis ground is 10 mil.


MID-2: System ground after magnetics only. No copper before the magnetics


Bottom Layer: LED control signals routed far away from magnetics and connector. otherwise no copper


  • \$\begingroup\$ You will need to provide many more details about your system -- please list all connectors, grounding scheme(s), test levels (emissions, immunity), and schematics and mechanical (assembly) diagrams. \$\endgroup\$ Commented May 8, 2023 at 18:01
  • \$\begingroup\$ "I have read a couple of application notes that advise the keep the system ground far away from the chassis ground." In a perfect world, sure. However, if your system has even modest external signal IO, then not likely. Then there's electrical safety issues which may require (or worse, forbid) this type of connection. It depends. Need details. \$\endgroup\$ Commented May 8, 2023 at 20:26
  • \$\begingroup\$ I have added screenshots of what I have right now to the question \$\endgroup\$
    – HV16
    Commented May 8, 2023 at 21:02
  • \$\begingroup\$ Okay, layout. What about schematics? What else connects to the board? What do the cables connect to? What standards must the project meet? \$\endgroup\$ Commented May 8, 2023 at 22:52

1 Answer 1


It depends, but also it probably doesn't matter.
For most of my RJ45, 10/100, or 100/1000 ethernets, I've connected the shield/chassis ground to my system ground using a 1M Ohm resistor and a 1nF capacitor, with a high voltage rating. I've got designs where I haven't or somewhere I've used a 10nF and I've never had an issue. The shield/GND connection isn't critical to the data.
RJ45 connection This is typical stuff for a RJ45, this is a 10/100. layout 100/1000 with the magnetics built into the jack. A keepout as the jack manufacturer prescribed but that's it.
100/1000 with discrete magnetics
In neither of the above designs do I have anything more than a trace connecting the shield GND to GND, or the taps of magnetics. These designs were short cables to other equipment sharing a common power source, so no particular need to worry about chassis GND. I wouldn't say that this is canonically OK, and possibly there are standards/best practices I'm not aware of that might be relevant to your project, but I'm saying they all worked no problem.
For the first few designs I was extra cautious, with keep-out zones under the magnetics and RJ45, but these days I don't bother with them. I'd still respect no copper zones as specified by the manufacturer of the RJ45 but that's about it.

If you're going to use 1M Ohm / 1 nF, then your layout spacing doesn't really as much. The tiny amount of conductance/capacitance (in comparison) isn't going to have much of an impact on these values. There is some logic in keeping the chassis GND to one side as it might be noisy, particularly if you're ethernet shield is connected to a long where, or your connector shares the enclosure chassis GND, but then you can always connect the chassis to the system GND in a more suitable fashion elsewhere.

As far as chassis GND vs other signals, then again, if I had genuine reason to think that chassis GND was going to be full of noise then it might give it space, but it also depends on how vulnerable the other traces are. A relatively high impedance trace to my ADC, yep keep that away. LED outputs, run them as close as you like, even if the noise was so gargantuan as to affect them, it wouldn't really matter as much.

It only really matters in the context of your larger system, and what this is going to connect to. If you're using an unshielded cable, then do whatever, but if you're connected over a long cable run to a different building then maybe look up the standard. Your PCB layout, and the tiny amount of capacitance/conductance, isn't as critical though.

  • \$\begingroup\$ have you got your boards test for EMI? I am more concerned about emission rather than signal integrity since it doesn't go to Gigabit Ethernet. \$\endgroup\$
    – HV16
    Commented May 10, 2023 at 20:32
  • \$\begingroup\$ No, none of these designs had to pass EMC. But integrated magnetic might be a good option for that as it simplifies things. Still, what you're connecting to, and how, is a much relevant as the layout. \$\endgroup\$
    – LordTeddy
    Commented May 11, 2023 at 11:12
  • \$\begingroup\$ It will be connected to an Ethernet switch. The cable has M12 connectors on the ends \$\endgroup\$
    – HV16
    Commented May 11, 2023 at 13:53

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.