Routing High Speed differential pairs across connectors / and or flex pcb. - Page 1
Forum section: electronics / projects

author: mrpackethead
author_rank: Super Contributor
timestamp: September 28, 2015, 12:57:58 am
content: I'm wanting to route 125Mz differential Signals ( ethernet ) between two pcbs that are 90 degrees opposed to each other.The options I can see(a) Create a Flex Rigid PCB that has ethernet signals that go across the flex to get to the other side. ( sounds like a chicken joke ).. The issue i worry about here is that theres going to potentially be some pretty ugly impedance mismatching going on across the flex, where the underlying material changes.(b) Use some kind of board to board connector, that will let me set up the 90 degree bend..Any body have any thoughts on this.

author: John_ITIC
author_rank: Frequent Contributor
timestamp: September 28, 2015, 02:47:50 am
content: Is this for a hobby or professional project? 125 MHz is not really high-speed so I would not worry too much about impedance mismatch and signal integrity issues. If you are in the multi-gigabit range then this becomes important. Make sure that you have a good ground plane under/next to the signals at all times. If using a flex cable, make sure you have ground signals next to the differential signals such that the loop area (and inductance) is as low as possible. Large loop areas mean lots of inductance and signal integrity and EMI issues.How about using a plain old PCI Express connector; the kind that is on a motherboard? That is intended to meet a plug-in card PCB at 90 degree angle. Those are also well designed with regards to SI/EMI and come in many different pin ranges.I have found that 2.5 Gigabit/second is quite forgiving, 5 Gbps starts to be tricky and at 10 Gbps you really have to know what you are doing!

author: marshallh
author_rank: Unknown
timestamp: September 28, 2015, 03:44:30 am
content: You can do that fine with 2layer flex. The substrates are very thin so the trace widths will necessarily be much thinner than FR4. Depends on your target impedance.Board to board connector is though. Like John said, pcie x4 connectors are commodity and if you can use them, do it.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 28, 2015, 04:05:11 am
content: Normal (single row) header stock is typically very similar to ribbon cable, i.e., 100-130 ohms differential (for any given pair, surrounding pins grounded), or ~50 ohms single ended (i.e., one line in use with the surrounding lines grounded).You can also get controlled impedance high-speed connectors (board-to-board and wire-to-board), but they're not worth it until you have long uncompensated LVDS signals, and gigabits. (100BASE-T is pretty tolerant of noise, though it's not frequency-compensating I think.)Flex can be had in controlled impedance, but it's probably not worth it. Board to board headers work pretty well.Best is always prevention, of course. Can you move the PHY up to the connector? Can you move the connector down to the PHY?Tim

author: mrpackethead
author_rank: Super Contributor
timestamp: September 28, 2015, 04:07:33 am
content: Quote from: marshallh on September 28, 2015, 03:44:30 amPCIE connectors are a pretty clever option. One i quite like. I'll have a look at that. 2 layer Flex is problematic. I need to carry a reasonable amount of current on the diff pair, ( i failed to mention it will have Power over Ethernet running ) as well. To get the target impednance matched for ethernet, the traces will so thin, that the current will fry them. rules that option out really.

author: mrpackethead
author_rank: Super Contributor
timestamp: September 28, 2015, 04:09:48 am
content: Really.. That would be a very simple solution, ( and cheap ).. its only 100Mb ethernet.. I can get the PHY pretty close to the transformer. (within about 10-15mm ) as the signal flys.Thanks. that would be awesome.Quote from: T3sl4co1l on September 28, 2015, 04:05:11 am

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 28, 2015, 04:12:58 am
content: If this has an external MII interface, remember that that should be impedance-controlled as well; but it only needs to be regular CMOS, and if it's point-to-point (from some controller or master device thing), a little resistor on each end will do (source termination). 50-100 ohm characteristic impedance, and matching resistors (don't forget to subtract the approximate Rds(on) of the CMOS output pins to get the required resistor value) should do the job, and with much more tolerance than the highspeed side.Tim

author: mrpackethead
author_rank: Super Contributor
timestamp: September 28, 2015, 04:39:09 am
content: Quote from: T3sl4co1l on September 28, 2015, 04:12:58 amRMII. So a few less connections. That bit is not problematic, since the Microcontroller and the PHY can be on the same pcb and very nearly next to each other. Still will all be matched. Its all on a 4 layer pcb, and the layer under neath those traces can be a ground plane.. ( will be a microstrip set up ).Pin header ( assuming i can get it to work ) would be so awesome, so it would work really well.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 28, 2015, 02:17:16 pm
content: Cool

author: mrpackethead
author_rank: Super Contributor
timestamp: September 28, 2015, 05:37:24 pm
content: Quote from: T3sl4co1l on September 28, 2015, 02:17:16 pmI really didn't think about using something as simple as pin header strip. I guess some days we overcomplicate things.

author: nctnico
author_rank: Super Contributor
timestamp: September 28, 2015, 06:26:50 pm
content: Quote from: mrpackethead on September 28, 2015, 04:09:48 amI'd be carefull with that. In many cases there has to be a certain distance between the phy and the transformer! A minimum of 25mm (1") isn't uncommon. Also don't forget TVS diodes and a couple of small ferrite beads (say 10 to 30 Ohm at 100MHz but do check their characteristic!) in series for EMC between the phy and the transformer. Regarding the connector: almost anything goes so a 2.54mm/0.1" header will do just fine. Most of the energy of a 100Mbit ethernet signal is in the first 10MHz or so.

author: mrpackethead
author_rank: Super Contributor
timestamp: September 28, 2015, 06:37:23 pm
content: Quote from: nctnico on September 28, 2015, 06:26:50 pmI have a similar design where the Phy and transformer is 16mm ( as the track flys ) away. It works well. The TVS diodes are critical! Learned that lesson the hardware a few years ago. Couldn't figure why my PHY's keep dying when i disconnected them from the PoE. I've been using Semtech R525S's for this purpose. Its actually on my list of things to research to replace, because the way it is packaged sometimes makes it hard to route the tracks without using vias. ( adding vias is a bad idea on these tracks ).. I think i'll be better off using single didoes or a package with two ( rather than package with four ).Obvisouly with a pin header, its likely that i'll end up with a connector that effectively has a right angle bend in it. That is something that we go to some lengths to avoid on these traces, but this might be unavoidable.

author: nctnico
author_rank: Super Contributor
timestamp: September 28, 2015, 09:53:21 pm
content: Wurth has nice dual TVS diodes for ethernet which are easy to route as well.

author: mrpackethead
author_rank: Super Contributor
timestamp: September 28, 2015, 09:58:24 pm
content: Did you have a part number for the wurth part? I had a look but I couldn't find anything. I'm a big wurth fan because they just are so easy to deal with.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 29, 2015, 01:01:19 am
content: Quote from: nctnico on September 28, 2015, 06:26:50 pmUh..Citation?QuoteUh, you might get away with that for RS-485, or even 10Mbps. But 100, uh, no.(And just to qualify that, in case you've "already done it, it works, I know": if you haven't measured the signal levels and edge speeds to be consistent with IEEE 802.3u specifications, and haven't tested its performance at full rated cable length and under EMC conditions, then you don't know how well "it works".)Tim

author: mrpackethead
author_rank: Super Contributor
timestamp: September 29, 2015, 02:05:26 am
content: QuoteThanks Tim. I feel so much better now. Another day of learning. Actually its really good, this thread has already been really helpful. As for thecertain distance thing. i've just got back and read the manufacturers notes for the Phy i'm using and it says, in the layout guide. it says"Place the RJ45 connector, the magnetics and the LAN9303 QFN as close together as possible."How would you recommend measuring the the signal level and rise/edge speeds?I was not sure about ntnicos comment about putting the ferrite beads in series, none of the reference designs i've looked at have those....the previous design was tested with 100m of Cat5 cable, and it "seemed" to work ok.. So, maybe i just got lucky.

author: John_ITIC
author_rank: Frequent Contributor
timestamp: September 29, 2015, 04:29:58 am
content: Quote from: mrpackethead on September 29, 2015, 02:05:26 amThe only thing this does is to remove the high-frequency content of the signal. This will lower EMI but also remove the quick edges of the signal!The correct way to lower EMI is to make sure that the loop inductance between the signal and return path is as small as possible. If using a differential signal then there will not be much EMI to worry about. This is because the return current will go in the opposite wire rather than in the ground plane. If your individual traces within the differential pair is not matched then you'll end up with EMI (due to a common-mode signal that will return via the ground plane) so make sure to length-match properly.

author: mrpackethead
author_rank: Super Contributor
timestamp: September 29, 2015, 05:29:41 am
content: Quote from: John_ITICThat is what i thought too..QuoteYes, trying to keep the traces as perfectly matched as possible. its not completely possible to keep them perfectly the same, but within 1-2%

author: NiHaoMike
author_rank: Super Contributor
timestamp: September 29, 2015, 05:52:02 am
content: Ethernet is very forgiving of imperfect wiring. Just look at the back side of one of those RJ45 wall sockets and you'll understand.

author: mrpackethead
author_rank: Super Contributor
timestamp: September 29, 2015, 05:58:27 am
content: Quote from: NiHaoMike on September 29, 2015, 05:52:02 amYes, and no...

author: nctnico
author_rank: Super Contributor
timestamp: September 29, 2015, 01:55:42 pm
content: Quote from: mrpackethead on September 29, 2015, 02:05:26 amFor some chips (IIRC SMSC) you have application notes for improving EMC performance. That is where you will find the series ferrite beads hint. EMC performance is not just affected by closely matching the impedance. At some point the ground plane is gone and you are left with a bunch of twisted pair wires. If the ethernet phy pumps out a lot of common mode HF originating from the modulation of the ethernet signals then the wires will be happy to act as an antenna. And if you look at the rear of an ethernet outlet you'll see the wires will be untwisted for quite a long distance. One of my customers uses a spring loaded terminal for connecting 100Mbit ethernet because it is more reliable than expecting electrical engineers to crimp an RJ45 properly onsite. That has been tested with maximum cable lengths, cheap switches, etc and it always works. I didn't expect that but if you look at transmission line theory you'll see that a small impedance discontinuity doesn't cause problems. For example: a lot of multi GHz RF chips don't allow to attach a microstrip of the proper width so there will be a discontinuity where the signal enters or exits the chip package but that isn't a problem.In my experience it is necessary to look closely at the application manual of the ethernet phy you are using but be aware not everything is in there and it may be necessary to add components which degrade it's signalling performance in order to pass EMC testing.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 29, 2015, 03:46:16 pm
content: Yeah, 100Mb isn't terrifically fast, so a short discontinuity doesn't count for much. You don't have to worry much about characteristic impedance if the PHY, transformer and connector are nearby.A ferrite bead is much very different than a few inches untwisted, though. For that to work, it would at least have to be a high frequency, low impedance type, not an average wideband 100 ohm (or whatever) type; in which case it wouldn't do much for EMC anyway.I wouldn't suggest playing with EMC on the PHY side, because it's supposed to be individual 50 ohm traces, not differential, at that point. (Except where the termination resistors join, which is 25 ohms Thevenin equivalent. Those should be right by the PHY to minimize stub lengths.)The magnetics handle EMC by using balanced matching transformers and common mode chokes. Additional ones could be added if there's imbalance at high frequencies (i.e., poor common mode rejection). You can get connectors with this built in, saving board area. They're actually fairly ugly inside (untwisted lengths, anyone?), but as long as it meets spec...Tim

author: mrpackethead
author_rank: Super Contributor
timestamp: October 02, 2015, 08:07:14 pm
content: once you've set up your scenario on a bit of board, and you plug it in and it "works", ( after following all the good information that has been suggestedby everyone, what is the sensible approach for measuring this and seeing how well it gets near to the standards