1
\$\begingroup\$

I'm laying out a PCB with 100Mbps Ethernet (SMSC LAN8710 Phy), a Pulse 1102FNL magnetics transformer plus the RJ45 [a MagJack isn't an option]. The transformer - probably as with most? - is 16 pin, with the RJ45-side Rx on pins 9/11 and Tx on 14/16. I appreciate that the diff pairs are important w.r.t. layout but there's also the centre taps, with their associated termination components. Is it best to keep these routed direct to the RJ45 pins, even if nestled between the Tx/Rx diff pairs, or to prioritise the diff pairs and route these taps around the sides etc? Ta enter image description here


Appreciate it's hard to review a screenshot, but here's a revised layout. The thick green line is the boundary between system ground and RJ45 chassis; the dotted green under the mags is a 'voided' area in the ground plane (not extended fully to the top of the mags because the right-hand diff pair is coming under and around). 'Bob Smith' components are R201/R204/R205/R206/C203.

enter image description here

The (blue) bottom layer tracks running horizontally are low-speed - drives to some/from LEDs, and a low-current tap off of the 3v3 rail.

\$\endgroup\$
  • \$\begingroup\$ If you have more information to add, don't post it as an answer. Edit your original question with the additional detail. electronics.stackexchange.com/tour \$\endgroup\$ – CHendrix Nov 2 '16 at 18:54
  • \$\begingroup\$ this design will have poor Return loss results @125MHz what are your specs? The pairs must be controlled impedance with ground reference \$\endgroup\$ – Sunnyskyguy EE75 Nov 3 '16 at 4:37
1
\$\begingroup\$

The priority is to optimize the routing of the tx and rx pairs. Run the pair 3-6 better.

I assume the magnetic has common chokes built-in, then the terminations to the unused pairs do not have much impact. So the routing of that would have the lowest priority.

Use thicker traces for the node where all the terminations go to the capacitor.

I remember 100Mbps Ethernet has a bandwidth of around 80MHz, so the wavelength over a trace would be like 2m. The short connections do not behave like transmission lines and it is not critical to get the exact trace impedance.

\$\endgroup\$
  • \$\begingroup\$ Thanks Rioraxe. Yep, the routing on 3&6 wasn't great in particular. As you've suggested, I've re-routed, taking the diff pairs (width/separation) as the priority. And yes, the mags [Pulse H1102] has CM chokes. It seems a general rule of thumb with discrete mags is to end the system ground plane on the Phy side of the mags, and have a separate 'chassis' plane under RJ45 and its side of the mags? (with option for 0R connecting the two planes, just in case) In which case the Bob Smith components should connect to system gnd rather than chassis? How about the 4 caps on the Tx/Rx signals? \$\endgroup\$ – ColH Nov 2 '16 at 16:11
0
\$\begingroup\$

You may consider locating each + and - differential signals' tracks as close as possible to each other. I would route it differently than you shown on the picture, having central outputs through via to termination circuit located on the other side of the board. I would also separated diff signals from other signals using GND polygons. There're other best practices like separating ground planes under the transformer, keeping digital signals like LED activity as far as possible from PHY circuit, but it is hard to advise without seeing circuit diagram.

You also may consider using MagJack connector with integrated transformer.

\$\endgroup\$
  • \$\begingroup\$ Thanks Anon. Yep - I haven't yet plugged in any ground plane separations. Would also prefer to avoid components on the reverse side [extra manufacturing cost]. (MagJack isn't an option because we need it do be a recessed/dropped RJ45 [Amphenol RJE72]) \$\endgroup\$ – ColH Oct 27 '16 at 15:59
  • \$\begingroup\$ Saving a cost now may cause product returns in the future. I hardly believe you can make it effectively mounting components only from one side. \$\endgroup\$ – Anonymous Oct 27 '16 at 16:09
  • \$\begingroup\$ I do take your point Anon, but we have no other need for dual-sided assembly anywhere else in the design, so it would be a shame to have to add to the manufacturing cost just for this area. Hence why I'm searching for a 'nice' solution :) \$\endgroup\$ – ColH Oct 27 '16 at 16:28
0
\$\begingroup\$

You have a 4-layer board, haven't you? If not, required track width/spacing makes this impractical – though I've once seen a USB2.0 Hub on a 2-layer board with 1mm track width/spacing on the signal paths.

Put the TX pair on the bottom layer, no other components near it. Of course, impedance-controlled. Keep the RX pair together, too, on the top side. Connect all other components as near to the transformer as possible, not the jack.

\$\endgroup\$
  • 1
    \$\begingroup\$ Janka, yes it's a 4-layer board. The track widths/spacings are being calculated for the correct diff impedance. \$\endgroup\$ – ColH Oct 27 '16 at 16:32

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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