6

I'm finishing off the layout of a board in Eagle which has a LAN8710A 100Mbps Ethernet PHY on it. The SMSC documentation is really pretty good but I'm stuck on the important detail of how to do the 100\$\Omega\$ differential pairs for the Rx/Tx. I understand this is important, but what I don't quite get is how to actually calculate the balanced impedance.

From what I understand, I can use this PCB Impedance and Capacitance Calculator (Microstrip) to calculate the characteristic impedance of the individual traces to make them 50\$\Omega\$, then use this PCB Impedance and Capacitance Calculator (Differential Microstrip) to calculate the differential impedance of the two tracks routed together. If this is wrong, please somebody point out my error.

However, the bit I don't understand is that both of those calculations require a distance to the ground plane. This is fine for the tracks from the PHY to the magnetics, but the SMSC app notes recommend no planes beneath the tracks from the magnetics to the connector, so how is this supposed to be calculated?

I'm confused. If someone out there can offer me some pointers it'd be much appreciated.

Greenonline
  • 2,064
  • 7
  • 23
  • 38
Redeye
  • 201
  • 3
  • 4

3 Answers3

4

Provide the right resistances on your side of the transformer and put the jack, transformer, and PHY as close as possible to each other. If everything is within a couple inches there is nothing to worry about.

Olin Lathrop
  • 310,974
  • 36
  • 428
  • 915
  • That's exactly what I'd done. Then I've read the component placement checklist for the LAN8710A and it says at least 0.5" between RJ45 and magnetics and at least 1" between PHY and magnetics. I wanted them a lot closer than that. So now I'm even more confused. – Redeye Oct 26 '12 at 12:36
  • @Redeye: Are you really sure it is specifying a *minimum* distance? If so, is any reason given? I can't think of why minimum separation would be required, except between the network and board sides of the transformer for voltage isolation. But, that's not what you are describing. Show a link to the datasheet that requires this minimum separation. – Olin Lathrop Oct 26 '12 at 13:01
  • Yes, it's definitely specifying a minimum. The document is here : https://www2.smsc.com/mkt/web_lancheck.nsf/e7c4b322c2cb1fbc85256d4e004dede3/fb7e94efd40b0dad852576650052a97b/$FILE/Placement%20Checklist%20for%20LAN8710%20QFN%20Rev%20C.pdf – Redeye Oct 26 '12 at 15:21
  • Sorry, should have said - it's on pages 4 and 5. The confusing bit is the first point says "put them as close together as possible". Then it goes on to specify minimum distances, but doesn't give any reason, although I've seen suggestions it's for EMI isolation elsewhere. – Redeye Oct 26 '12 at 15:23
  • @Redeye: I see what you mean, but it doesn't make sense to me either. They are quite explicit about it though, so it's not a typo or bad wording. You might want to inquire from a FAE what exactly the purpose of the minimum spacing is. If you find out, it would be good to append the information to your question. – Olin Lathrop Oct 26 '12 at 15:41
  • 1
    I've asked the question, I'll see what they come back with. So, to the other part of my question - how do you calculate differential impedance when there's no ground plane to put into the equations for the return path (ie. between RJ45 and magnetics)? – Redeye Oct 26 '12 at 15:54
  • I have seen people cut out ground planes under the entire path (myself included) but you violate the spec if you don't properly terminate, which you can't do without a ground plane. I've started using the CGND plane (or whatever is shielding your cable) from connector to transformer then a DGND plane from transformer to PHY. Most importantly though, make sure you match the lengths of the traces to keep skew down. When I am directed to remove planes completely, I follow Olin's advice of shortest lengths possible. – Analog Arsonist Oct 26 '12 at 16:55
  • So, I basically have the choice of ignoring the manufacturers recommendations which makes more sense to me, or sticking to them despite that meaning that I can't see a way to calculate the differential impedances with no ground plane underneath. Not an easy choice... – Redeye Oct 26 '12 at 21:39
  • @Redeye “how do you calculate differential impedance when there's no ground plane to put into the equations for the return path (ie. between RJ45 and magnetics)?” Yes, differential signal does require ground between tx and rx for common mode voltage within specification, but differential impedance calculation does not. For model purpose, you just use the model without ground, if the model requires you somewhat input an H1, just make it 20x of S1(trace separation), as said in "polarinstruments.com/support/si/AP8153.html". – iouzzr Sep 27 '18 at 06:52
  • @Redeye There are two cases to consider: 1. Most return current is carried by the plane when trace to plane coupling >> trace to trace coupling, Ex most board level interconnects. 2. Most return current is carried by the other trace when trace to plane coupling << trace to trace coupling, Ex most connectors, shielded twisted pair, twisted pair. I find all this information online, because I have the same questions, hope this will help, after all these years. – iouzzr Sep 27 '18 at 06:56
3

If you have to use separate magnetics then you could use the same basic spacing and trace widths from the magnetics and over to the RJ45 as you used for the Diff Pair coming from the PHY. Do keep the jack end of the magnetics component as close to the RJ45 as possible.

Note that if you were to use a MagJack (which is an RJ45 with the magnetics built in may be somewhat easier to deal with. Some of these MagJacks require the addition of some components near the RJ45 that get referenced (and/or connected) to a copper pour around the connector pin area. It is common that this pour also have a cutout under it in the PWR and GND layers.

Michael Karas
  • 56,889
  • 3
  • 70
  • 138
0

You need to contact your PCB manufacturer to find out what the board stackup is. Then you will know the distance to the ground plane and therefore can set the track width and separation in order to meet the required impedance.

Hefin
  • 1
  • Welcome to EE.SE. OK answer but missing details and links to answers with similar problems. When answering questions check right-most column for 'related' articles. –  Jul 28 '16 at 17:14