1
\$\begingroup\$

I am designing a Ethernet PCB with external magnetics on a 4 layer board. On the PHY side I have the system ground on the adjacent layer under the two differential pair for the return path. How about in between the connector and the magnetics? Should I pour a chassis ground plane under the traces or am I not suppose to have any copper?

\$\endgroup\$
1
  • \$\begingroup\$ Do you need L2 copper to obtain the correct trace impedance? If you do, the chassis node is the only sensible choice. Provide enough clearance to the system ground. Best is to keep this very short and use no L2 copper IMO. \$\endgroup\$
    – tobalt
    Commented May 3, 2023 at 3:58

1 Answer 1

2
\$\begingroup\$

I suppose the first point that comes to mind: it may be difficult to achieve isolation requirements, pouring ground under the media traces [on nearest mid layer]. That said, you could still use the "Bob Smith" common node (to which the unused pairs, and center-taps, are terminated, with the 1nF to ESD ground) as a ground plane for these.

You generally won't want to route media traces as diff pair without ground, as the impedance will be too high. Edge-coupled traces with ground, couple poorly to each other; even without ground, they still couple poorly, requiring large trace widths for impedances like this. You can however route them top-mid or top-bottom as broadside-coupled pairs, which will see a more modest trace width.

Finally, if there's very little distance between connector and transformers -- mismatch really doesn't matter. And since conventional 100/gig Ethernet only uses around 100MHz bandwidth, "little" is perhaps 10cm or less. Ethernet may be high bandwidth in relative terms, but it's nowhere near as intensive or demanding as a DDR3+ or PCIe interface is!

There is also an argument to prefer the no-ground case in terms of common mode impedance: we're probably not talking much coupling distance here (i.e. maybe some ~cm of pair over plane, wired to whatever ground return you choose), so again it doesn't matter much, but the case could be made that no-ground is preferable as it's consistent with the environment of the cable itself. That is, you can avoid introducing more and longer impedance discontinuities. The connector and transformer are already two, and coupling the pair to a ground adds a third. Discontinuities mean more impedance changes vs. frequency, and maybe that worsens CMRR at some frequencies.

Or conversely if shielded cable and connector are in use, extending that shield onto the board (and tying the "Bob Smith" node to it) would be equally logical.

To be clear, chassis ground is most likely the "ESD ground" mentioned above, i.e. where the "Bob Smith" common node should be bypassed to. Because of isolation requirements, chassis ground probably shouldn't be used for this directly, but due to the capacitor, these two nodes will have similar RF voltages.

\$\endgroup\$
6
  • \$\begingroup\$ Many good options here: Bob Smith GND capacitively connected to the Chassis/Shield node or no pour with broadside coupled traces for larger isolation if necessary or if there is no BS available from the magnetics. \$\endgroup\$
    – tobalt
    Commented May 3, 2023 at 7:08
  • \$\begingroup\$ the physical distance between the connector and the magnetics is half an inch. I am using an M12 connector with two pairs; I use Bob Smith to tie the center tap of these pairs to "ground" (not exactly sure how this ground get connected). The cable and connector are shielded and have metal contact with the chassis. Based on your comment, if I understand it right: the distance is too short to cause any issue; however, since the pairs are shield, it is better to have a ground plane underneath them on the PCB. \$\endgroup\$
    – HV16
    Commented May 3, 2023 at 7:38
  • \$\begingroup\$ so I guess what needed to be done is, have a copper plane underneath the differential pair, this plane is tied to Bob Smith ground, then capacitively connect Bob Smith ground to chassis ground. \$\endgroup\$
    – HV16
    Commented May 3, 2023 at 7:40
  • \$\begingroup\$ @HV16 Quite correct! \$\endgroup\$ Commented May 3, 2023 at 9:31
  • \$\begingroup\$ @TimWilliams Great! Do I also have the place a capacitor between system ground and chassis ground, or system ground and magnetics ground? And should I keep a big distance between the system ground and the other two? How about magnetics ground and chassis ground? Do they also need to be physically separated? \$\endgroup\$
    – HV16
    Commented May 3, 2023 at 21:09

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.