Long trace high-speed connector board - Page 1
Forum section: electronics / beginners

author: jtvo
author_rank: Newbie
timestamp: June 12, 2023, 05:46:56 pm
content: Hi, first time posting, thank you!I am traditionally a mechanical designer and need to create a PCB (or multiple) that will run standard computer connections about 20cm from one side to another: 24pin atx power,(2) 8pin atx power, 4pin atx power, HDMI 2.2,(2) Displayport 2.1, Ethernet,(6) USB 3.0+, and (3) SATA 3.0 data. Attached are some pictures of the master board we already designed.I'm getting a lot of conflicting feedback as to if it would work or not. I was hoping to get some clarity and my questions are as follow:1. Is an exotic material required for this board to function properly? Rogers 4350B, Megtron6, etc.? I have been told that my specs require 12ghz frequencies and FR4 can't keep up.2. Is having all of these connections/traces on one board wrong? Should I split them into separate boards due to interference and grounding issues from the 24/8pin atx power to ethernet to hdmi/displayport, etc.? How many boards? Should ethernet be isolated on its own board?3. Is a redriver required for these trace lengths on the HDMI/Displayport signals?4. Are through-hole connectors disqualifying for these signals due to increased losses?As of now, I'm leaning towards splitting off the power lanes into a separate board as one should be able to build in FR4 material for power, right? The rest is a toss-up and I need some guidance.Ideally, the data connections would all sit on one or two boards; especially if one could be made from a relatively low cost material.Thank you for your help!Best,JTvo

author: jtvo
author_rank: Newbie
timestamp: June 12, 2023, 09:33:09 pm
content: I should mention that the designer and I spoke ad-nauseam about trace length impedance matching and supposedly that has been considered in the design.

author: jtvo
author_rank: Newbie
timestamp: June 14, 2023, 04:38:25 pm
content: Bump**Is there a more appropriate forum for me to post these questions?Thank you

author: dmills
author_rank: Super Contributor
timestamp: June 15, 2023, 08:33:04 am
content: It is the sort of thing where you either need to build it and measure the performance, or get into some very expensive simulation games.My experience is that reclockers are always a good idea behind a connector, almost irrespective of board material because the connectors tend to be 'interesting' from a RF perspective.How many layers are you using, and what does the stackup look like?The ethernet is pretty much easy here, it is after all specified to work over 100M of cable, which makes a competently designed set of pairs on a board look harmless in comparison, is is also (assuming 1 Gig) only 125MHz DDR on all pairs, so meh.The video ports are the ones that would worry me, because those barely work properly on a good day, and are screamingly fast, and a reclocking driver here would not hurt anything.The USB3 pairs are another one to watch, but note that many so called USB3 ports actually only connect the USB2 pair, which is comparatively slow (480Mb/s), note that there are traps here in terms of getting good EMC performance because USB is neither fish nor fowl when it comes to the question of single ended Vs differential signalling and there is some very dubious advice floating around as to how to connect the grounds at the connectors.The quick stuff (video, USB3 data, and maybe the sata) should probably use SMT connectors (with tabs to make them less likely to get pulled off) to avoid the need for back drilling or other suchlike nonsense, but that (and the question of what material to use for the layers in question) very much depends on either measurement of simulation (Very expensive software involved here).Given the low cost of spinning an FR4 prototype I would probably do that and measure the resulting eye for each signal, it is not like you are especially likely to get it all perfect on the first shot even if you use expensive substrates.You will very obviously need a ground plane, and it feels like at LEAST 4 layers to get the plane close enough to the signal layers to make the impedances work at sane trace widths.Final question : Where are the mounting holes? Do NOT rely on connectors to mount this.

author: jtvo
author_rank: Newbie
timestamp: June 15, 2023, 08:32:36 pm
content: Thank you so much for your response!4 layers and 35/18/18/35 is the stackup. The mounting holes are around the edges, note the attached split power board. I have a gasket running around the top of the connectors as there is liquid inside the container.The video ports are the most concerning as I barely understand them (I've built a variety of USB and Ethernet cables).We designed with through-hole connectors, and will switch to smt. Do you suggest smt for all the data connections or just video?Considering this redriver, though would prefer to avoid if possible.https://www.nxp.com/products/interfaces/high-speed-signal-conditioners/20-gbps-per-lane-4-lane-displayport-linear-redriver:PTN3816Moving forward, I'm going to split this into 2 or 3 boards and use an expensive substrate for the HDMI/DP board. I had size constraints fitting all my connectors onto one board and now could shorten the video board if that relieves the redriver requirement.I had just heard one could send HDMI or DP over USB C. Is that easier to make long traces for?

author: radiolistener
author_rank: Super Contributor
timestamp: June 15, 2023, 11:30:53 pm
content: Quote from: jtvo on June 12, 2023, 05:46:56 pmYes, through holes affect transmission line performance, but not because of losses, but due to non-constant impedance along the transmission line and impedance mismatch. The same wire geometry, copper thickness, PCB material and PCB thickness and layer thickness also affect it. So all these parameters should be taken into account when you design PCB.You're needs to know PCB material properties and copper thickness in order to calculate wire thickness and distance between wires for specific impedance.PCB solder mask and silkscreen material also affects impedance, especially for signals above 500 MHz, if you're dealing with such frequency, then you're needs to request PCB manufacturer to use special RF-grade material for solder mask and silkscreen which has stable electromagnetic properties which you can use for wire geometry calculations. If transmission line is very sensitive to impedance, it's better to not use solder mask and silkscreen above transmission line at all.