EEVblog Electronics Community Forum
Electronics => Projects, Designs, and Technical Stuff => Topic started by: philby on May 23, 2022, 12:03:31 pm
-
I am hoping to get some insight from experienced electronics engineers on signal integrity over regular PCB header strips.
Long story short, In a PCB design I am working on I need move the ethernet RJ45 port from my mainboard onto a mezzanine card.
The PHY and magentics will remain on the main board. The 4 differential pairs (Gigabit speed) will connect up to the RJ45 on the mezzainine card.
I am hesitant to use a high speed mezzanine card like the edge-rate from semtec (https://www.samtec.com/connectors/backplane/micro-backplane-systems/edge-rate#series (https://www.samtec.com/connectors/backplane/micro-backplane-systems/edge-rate#series)) because
• I want to avoid placing SMT parts on both sides of the board
• The cost. The board has 5 ethernet ports and am on a tight budget
Ideally I would like to use regular PCB header strips (https://www.samtec.com/products/matedsetinfo?male=MTSW-104-07-L-D-165&female=SLW-104-01-L-D (https://www.samtec.com/products/matedsetinfo?male=MTSW-104-07-L-D-165&female=SLW-104-01-L-D)) since
• They can be easily hand assembled on the rear of the board.
• They are very cheap
Am I likely to introduce serious signal integrity issues using the regular PCB header strips? Maximum length of ethernet cables in the system will be about 5 meters, so I am hoping the short cable run will give me some signal quality headroom to do something sub-optimal on the PCB. My gut feeling is it will work ok, but I am hoping someone more experienced can offer some insight.
-
Non-optimal situation can be improved by having ground pins close by the signal pins, to give reference plane - like was done in ribbon cable to interleave signal and gnd for improved performance. Also, when a faster connector is inevitable, don't forget there is PCI-e -> comes in different sizes; only one connector needed, other side comes from pcb itself; made for high speed signals / controlled impedance; mass market part with corresponding price. To give indication on impedance discontinuity, make a prototype and measure it with VNA (bonus points if VNA has TDR option, you'll be able to see precisely then)
-
Non-optimal situation can be improved by having ground pins close by the signal pins, to give reference plane - like was done in ribbon cable to interleave signal and gnd for improved performance. Also, when a faster connector is inevitable, don't forget there is PCI-e -> comes in different sizes; only one connector needed, other side comes from pcb itself; made for high speed signals / controlled impedance; mass market part with corresponding price. To give indication on impedance discontinuity, make a prototype and measure it with VNA (bonus points if VNA has TDR option, you'll be able to see precisely then)
Thanks ch_scr.
Yes. Having adjacent ground pins to high speed signals will help with signal integrity. Since this is ethernet, it is just the differential signals. I would keep differential pairs on adjacent pins.
I had not considered PCI. I'll do some investigation thanks.
I don't have a VNA, but I think I can get my hands on one for some testing. Thanks for the suggestion.
-
I find the networking stuff pretty forgiving; grounding between the signals and a grounded metallized foil around the cable, that should easily be good enough for 1Gbit.
-
flip your mezzanine card upside down... many of the samtec connectors are available in multiple heights.
-
flip your mezzanine card upside down... many of the samtec connectors are available in multiple heights.
Thanks for the suggestion free_electron. Normally I would but due to some thermal management considerations that is not an option in this instance.
-
Is this after PHY/magnetics so it's just the naked (media) pairs? Not even anything to ground then? The main thing you get is the uncoupled length of the header itself, which isn't even that poorly matched (probably somewhat over 100 ohms for 0.025" sq post x 0.1" pitch?), and whatever DM coupling you might get to nearby structures (so, if the headers are by themselves off to the side, say, they're probably fine).
Headers certainly aren't any worse geometry than the mod connectors themselves, or the cable joins/boxes installed throughout a facility. Ethernet is quite forgiving as its bandwidth isn't as serious as you might think (400MHz) so it's quite tolerant of uncoupled/mismatched/stub lengths, and, I forget which modes employ reflection cancellation and such (not 1000BASE-T I think, probably the higher ones??), but that's a thing too, when it is. Basically it's made to handle awful conditions. Not that you should be careless on-board, you don't want to use up that tolerance budget all at once, of course.
Tim
-
Gigabit Ethernet is only 125 MHz and pretty tolerant of reflections. You will probably be fine. Adding grounds between adjacent pairs will reduce crosstalk even if you just connect to a small ground polygon on the board, but probably isn't necessary.
Can you use magjacks instead so the connector goes between the phy and the magnetics?
-
Ah right, it's the one 10G over copper that's 400MHz actually, and gig isn't even that, it's 62.5MHz (125Mbd) over 4 pairs. Basically 100BASE-T with better coding (more levels per symbol) and only slightly higher rate:
https://en.wikipedia.org/wiki/Gigabit_Ethernet#Copper
https://en.wikipedia.org/wiki/10_Gigabit_Ethernet#Physical_layer_modules
(There are also standards for 1-2 lane half/full duplex, usually for automotive (entertainment systems etc.). Obviously, those have to run much faster for the same total rate.)
Can you use magjacks instead so the connector goes between the phy and the magnetics?
Think I'd rather have media than PHY over the headers -- but the "full bridge" style driver typical of (most? all?) gig PHYs should be more tolerant of that than 10/100 (which typically use a CT winding and push-pull drive). Which even then, again, hardly matters because the permissible stub length is so long (10s cm?).
...I wish that Ethernet qualification/testing tools were more common/accessible(/affordable?); it would be nice to see even just a comparison of these effects in circuit. It's one thing to say: "minimize stub lengths", it's something completely different to say: "keep stub lengths below X to maintain +/- 0.YYY dB of specified frequency response". I don't recall ever seeing such a comparison in appnotes (which, appnotes, that's par for the course).
Tim
-
Also keep in mind 1000BASE-T is defined for cables as long as 100m, and a fully compliant connection must fulfill that. But for cables of a few meters only, as the OP stated, you have a lot of leeway.
-
Is this after PHY/magnetics so it's just the naked (media) pairs? Not even anything to ground then? The main thing you get is the uncoupled length of the header itself, which isn't even that poorly matched (probably somewhat over 100 ohms for 0.025" sq post x 0.1" pitch?), and whatever DM coupling you might get to nearby structures (so, if the headers are by themselves off to the side, say, they're probably fine).
Thanks Tim,
My plan was for just naked pairs to the mezzanine card. Nothing referenced to ground going over the connector.
Headers certainly aren't any worse geometry than the mod connectors themselves, or the cable joins/boxes installed throughout a facility. Ethernet is quite forgiving as its bandwidth isn't as serious as you might think (400MHz) so it's quite tolerant of uncoupled/mismatched/stub lengths, and, I forget which modes employ reflection cancellation and such (not 1000BASE-T I think, probably the higher ones??), but that's a thing too, when it is. Basically it's made to handle awful conditions. Not that you should be careless on-board, you don't want to use up that tolerance budget all at once, of course.
Tim
Yeah. That is what I am thinking too. I just don't want to end up with a dead board. The micro and ethernet switch IC's have been almost impossible to source. Last thing I want to do is waste what little stock I have been able to secure on dud prototypes.
-
Another option worth considering could be using FFC jumpers. They're fairly cheap, high signal density, and you get enough positioning flexibility that you could probably find a way to route the jumper(s) to a connector on other side of the board. Controlled impedance FFCs are available ($$$) but the differential impedance of standard polyester 0.5mm FFCs is about 100R: https://meritec.com/wp-content/uploads/2014/03/FFC-Impedance-Tests.pdf (https://meritec.com/wp-content/uploads/2014/03/FFC-Impedance-Tests.pdf) Of course the pairs aren't twisted, so coupling to anything else in the box is more differential and less common.
On the subject of dealing with non-ideal wiring for Ethernet, the attached photo is from the inside of a Neutrik NE8FF etherCON coupler (https://www.neutrik.us/en-us/product/ne8ff), which uses a pair of small PCBs to adapt the connectors on the ends to pairs of two-core zip wire that go between them. Note the little interdigitated PCB capacitors that they've included for impedance compensation. So, you know, you could always carefully analyze the impedance of your connector solution and your PCB stackup and calculate some incredibly fussy compensation structures to design into the board. Or you could just use the header pins as they are and, with a little bit of care, probably never have a problem with it :P
-
Another option worth considering could be using FFC jumpers.
On the subject of dealing with non-ideal wiring for Ethernet, the attached photo is from the inside of a, which uses a pair of small PCBs to adapt the connectors on the ends to pairs of two-core zip wire that go between them. Note the little interdigitated PCB capacitors that they've included for impedance compensation. So, you know, you could always carefully analyze the impedance of your connector solution and your PCB stackup and calculate some incredibly fussy compensation structures to design into the board. Or you could just use the header pins as they are and, with a little bit of care, probably never have a problem with it :P
Thanks ajb. I was just discussing FFC with the team yesterday if the current solution doesn't pan out. I just sent the board away for fabrication so fingers crossed.
Regarding the picture, I love this sort of design. It's that kind of thinking that can get you over the budget line. Thanks for sharing.