0
\$\begingroup\$

While working on a new design, we had to route Ethernet signals on our PCB. My colleague and I has some discussion on how we should handle the grounding around the Ethernet signals, and their return path.

The signals are routed from the PHY to the magnetics, travel some distance on the PCB, and exit through the Ethernet connector. Our discussion was for the part after the magnetics and up to the connector.

My colleague proposed that we shall add a proper ground plane under these signals, and pay attention to the return paths.

I, on the other hand, proposed that we don't need this, as the Ethernet signals are magnetically coupled, and essentially galvanically isolated. Its like having an unrelated cable just happening to be close to the PCB, without any actual electrical connection.

So, is it actually needed to have a return path for the Ethernet signals?

\$\endgroup\$

2 Answers 2

1
\$\begingroup\$

You are correct, you do not need a return path for the signals between the magnetics and RJ45 jack. To quote from the SMSC (now Microchip) app note:

Under no circumstances should a ground plane exist under the magnetics, the RJ45 connector, or in between the magnetics and RJ45 connector.

This is visible below (from the same source):

PCB from app note

The "disagreement" around this area is to do with the optimum way to comply with the ethernet standard (802.3) regarding electrical isolation, and the minimisation of EMI to within acceptable limits.

\$\endgroup\$
0
\$\begingroup\$

It could be argued that the return path in a differential pair is the other trace, but the ground plane is still needed to get impedance under control because edge coupling is too weak (but it needs to be taken into account for the geometry calculation of the microstrip).

It doesn't even need to be a ground plane, an otherwise unconnected plane will do as well, since the plane is not connected to the magnetics anyway. The place where the differential pair connects to the components will be a discontinuity both on the top layer where the geometry is given by the solder pads and the component pins, and on the bottom where the return paths are terminated with a too-small resistor, but this is usually okay.

In theory it is also possible to route the pair on different layers, but it is uncommon because you still need two layers, same as for edge-coupled microstrip, so you don't gain anything on a two layer board, and on boards with more layers you need to stay away from this transmission line on all layers, while a microstrip on top would be reasonably shielded from whatever is going on at the bottom by a ground plane on an inner layer.

\$\endgroup\$

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.