14
\$\begingroup\$

This is my first 100 Mbit/s Ethernet project (I am doing it to learn more about differential signals).

I did two things that I don't know if are good or bad in this particular case.

One is to route under the signal transformer. It is only slightly on the border, but I didn't find any other way to route it, without using vias to swap the pair.

What do you think? It would be better to use vias (and an impedance mismatch), or route so close to the inductor?

Also, I tried the differential tools in KiCad, and I matched both pairs to the same length (otherwise, one track is about 6 mm longer). Is this a good practice for Ethernet?

This is a capture of the PCB right now:

Enter image description here

This is the schematic that I am using. It uses the lan9512 reference schematic. To be honest, I am no idea of the impedance on my design. I am not sure if I have to use 50 ohm or 100 ohm.

Enter image description here

I include the impedance calculation for a double sided PCB, FR4 1.6 mm height and 1.6 oz copper (35 µm)

As you can see, the track with is 0.8 mm!! - way too large.

Enter image description here

This is the final version. Track with 1.6 mm, gap 0.16 mm (minimum in my cheap PCB provider).

Enter image description here

Thank you everybody for this valuable master class. I will read a lot about differential pairs.

\$\endgroup\$
  • 1
    \$\begingroup\$ Is data polarity important to maintain in ethernet? \$\endgroup\$ – Andy aka Apr 29 '16 at 11:18
  • 1
    \$\begingroup\$ How about the reversal happens on the other side of the transformer? \$\endgroup\$ – Andy aka Apr 29 '16 at 11:45
  • 1
    \$\begingroup\$ good question, can I swap RX- and RX+ and CRX-/CRX+ in my schematic? \$\endgroup\$ – Javier Loureiro Apr 29 '16 at 11:47
  • 1
    \$\begingroup\$ @michael: because my plan is to use 4 ports in the next version, and i didnt find 4 port magjacks at a reasonable price. \$\endgroup\$ – Javier Loureiro Apr 29 '16 at 11:59
  • 1
    \$\begingroup\$ I would still use MagJacks and just put four of them side by side. \$\endgroup\$ – Michael Karas May 1 '16 at 11:14
12
\$\begingroup\$

If I were to suggest how to route this I would propose something more like this:

enter image description here

\$\endgroup\$
  • 1
    \$\begingroup\$ Clever picture editing gets my vote. \$\endgroup\$ – Andy aka Apr 29 '16 at 12:39
  • 5
    \$\begingroup\$ Definitely agree, length matching is only half the battle with diff pairs. If you have the same length traces but each takes a radically different route across the board then it's quite possible for one of the traces will be subject to inductive/capacitive (etc) effects that the other trace is not. @MichaelKaras' suggestion is preferable, because any inductive effects will be experienced equally by both traces and will be cancelled out by the way that diff pairs intrinsically work. \$\endgroup\$ – Wossname Apr 29 '16 at 12:49
  • \$\begingroup\$ I see. the transformer could affect both traces, but the effect wont cause mayor problems. +1 \$\endgroup\$ – Javier Loureiro Apr 29 '16 at 13:27
3
\$\begingroup\$

About impedance: you clearly need 100 Ohms differential, it is the same as 50 Ohms single wire. You have to use some "impedance calculator" (for example: https://www.eeweb.com/toolbox/microstrip-impedance). The dielectric thickness goes from your PCB design. The copper thickness is typically 35 um, it has a little effect on results. The trace width and trace separation does matter for RF designs.

\$\endgroup\$
  • \$\begingroup\$ Another good tool is Saturn PCB Toolkit. \$\endgroup\$ – rdtsc Apr 29 '16 at 12:14
  • \$\begingroup\$ Interestingly, USB2.0 and Ethernet (10/100 at least, not sure about GBE) have very similar characteristic impedance requirements, which makes life easier when you have both on a single design. In my experience USB2.0 needs 90 Ohms +/-15% and Ethernet typically is around 100 Ohms, there is a handy window of overlap there. \$\endgroup\$ – Wossname Apr 29 '16 at 13:02
  • 1
    \$\begingroup\$ Also, you can always ask your board manufacturer to do the impedance calcs for you when you submit the Gerbers to them. This is a standard thing to ask for and they won't charge you for it (most likely). In fact you can even ask them to change the trace width for you in order to meet the impedance you want. \$\endgroup\$ – Wossname Apr 29 '16 at 13:10
2
\$\begingroup\$

About length matching: This is not as important as one might think. 100MBit Ethernet uses a symbol rate of 125 MBaud/s, each symbol is 8 ns long. Compared to that, a 10 mm different routing length introduces a skew of (speed of signals in copper traces is roughly half the speed of light) 30 ps only, or less than 0.5%. While this slightly reduces the margin to get bit errors on the receiver, the influence is negligible.

I would rather focus on providing (roughly) the correct impedance. Without going for more expensive impedance controlled PCBs, the best rule of thumb is: Distance between both traces should be the same as their width and the distance to the next ground layer should be a bit more than the width of the two traces. E.g. 150um traces, 150um gap, 200-400um to ground layer (as is typical on a 4 to 8 layer PCB).

\$\endgroup\$
  • \$\begingroup\$ Ok, thank you, this answer helps me a lot!! This board is only 2 layers (I believe that 4 layers is way better, but this is only a test for myself). I am planning to dont use a ground plane under all differential traces (even usb ones). \$\endgroup\$ – Javier Loureiro Apr 29 '16 at 13:30
  • 4
    \$\begingroup\$ I strongly advise to use ground plane below high speed traces. \$\endgroup\$ – Master Apr 29 '16 at 15:08
  • \$\begingroup\$ @asdfex, I use 0.1 mm FR4 between Top high speed lines and next ground plane. The trace width for 50 Ohms (as I remember) is 0.16 mm. This works fine, I ordered impedance control several times - no need to change the width. The differential 100 Ohms line has width 0.15 mm and separation 0.15 mm. Using 0.2-0.4 mm dielectric leads to too thick PCB, even on 8 layers. \$\endgroup\$ – Master Apr 29 '16 at 15:15
  • 1
    \$\begingroup\$ @Master Your differential 0.15/0.15 traces and 0.1mm dielectric gives about 80 Ohms impedance. My 0.15/0.15 and 0.2 yields a close to perfect 95 Ohms, even better with 0.1mm traces and gaps. My PCB producer has a default 8-layer stack of 180um separation between each of the layers, at a total stack height of 1.6mm. \$\endgroup\$ – asdfex Apr 29 '16 at 15:42
  • \$\begingroup\$ @asdfex, did you measure the impedance or did you order the impedance control manufacturing process? I really wonder. The difference between your design and my design is, say, rather large. My design is not only based on calculations, it is verified several times by the impedance control process at PCB manufacturer. They told me no need to change the width as the impedance is 100 Ohms within few percent. \$\endgroup\$ – Master Apr 30 '16 at 15:31
0
\$\begingroup\$

At the lengths and the speeds your board will see, it probably won't make much difference. At 100Mbit that's only 50MHz of bandwidth, length matching traces is usually not an issue until the length difference becomes a meaningful fraction of the wavelength (which at 50MHz is 6 meters, even the 9th harmonic is still over half a meter). I wouldn't worry about it.

\$\endgroup\$

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.