USB 3 question - Differential lines length - cables? - Page 1
Forum section: electronics / projects

author: timgiles
author_rank: Regular Contributor
timestamp: March 25, 2016, 10:03:19 am
content: Hi all,I am in the middle of designing a USB 3 4 port hub. In the TI datasheet for the hub IC, it advises that the differential lines for the USB 3 RX and TX pairs must be of similar length, + or - 5mils. USB 2 data lines, + or - 50 mils.So I can understand why this is, as there is unlikely to be much in terms of a buffer and the incoming signal needs to be matched for error correction. However what I dont understand or its hard to believe is that the USB 3 cables I buy are made to this tolerance. Is it right that the individual wires inside USB 3 cable are cut and soldered to a tolerance of +/- 5 mils (or just over 0.1mm)!!??If not, then why is it so important on a hub PCB for the traces to be so close in length but not the cable? If it is the case, how do they mass produce a cable with wires soldered in place so accurately?Thanks for your time

author: timgiles
author_rank: Regular Contributor
timestamp: March 27, 2016, 08:26:18 pm
content: After some googling - found thishttps://www.ieee.li/pdf/essay/differential_signals.pdfwhich gives a good explanation - in case others are interested.

author: marshallh
author_rank: Unknown
timestamp: March 28, 2016, 05:37:20 am
content: USB3 and other similar modern serdes-based interfaces (like PCIe, SATA, etc) operate with independent differential lanes. Only worry about difference between +/-. All sorts of magic is used to open back up the eye at the receiveing end, like sending a long pattern of known values to calibrate the receiver when bringing the link.There is a certain amount of timing "budget" designed into the spec. For the distance you run the lines on a lossy medium like FR4 or each time you have an impedance discontinuity it eats up part of that budget.What's far more important than worrying about the inter-pair length matching is ensuring the lines have consistent impedance throughout. Calc your trace width given the pcb stackup, and make sure the lines do not pass above any slots or breaks in the current return path (at 5gbps, it is a fuzzy line in the ground plane underneath the data lines).Try to match the specs as much as practical, but don't sweat it - I've seen truly horrific 3.0 hubs with 2layer pcbs and multiple slots, and it still worked (poor budget was about toast though)

author: timgiles
author_rank: Regular Contributor
timestamp: March 28, 2016, 01:27:28 pm
content: Thanks Marshall,I now feel the same way, I will do my best to follow the suggestions but not sweat too much blood over it. I have taken a look at the 4 port reference design TI have on their website - and it is clear that they route differential pairs near each other without detrimental effect. Yes - I have used an online calculator and got as close to the recommended impedance as I can. After all the reading its a lot clearer in my head as to why TI state what they do.Regards Tim

author: Apollyon25_
author_rank: Regular Contributor
timestamp: April 01, 2016, 03:02:40 am
content: Altium has length tuning tools, so this is actually quite easy.Just route these lines first and make everything else fit around the diff pairs.As long as you route with (I know USB2 is 90/45 ohms...) appropriate trace impedances, and have the D+/D- lengths matched, you'll probably be fine. And if you can do this, you can equally easily match the pair lengths.If you intend to sell this, then you will need to try to meet the layout recommendations as well as possible. Diff pairs are very prone to DM-to-CM conversion and cause EMI/EMC issues.USB.org have test meet-ups (but being in NZ, I havent been able to use this)If you have a professional EE CAD software package you should have no trouble.Also, there's a high speed diff pair routing tutorial video on YT from a TI guy, that's pretty good.