5
\$\begingroup\$

Properly routing USB, DVI and Ethernet signals over long distances (30 to 40 cm) on a PCB seems to be relatively challenging (skew, characteristic impedance, cross-talk, etc.). Yet using the standard off-the-shelf cables appears to allow proper signal transmission over meters without putting too much thinking into the design. (see for example USB tech doc suggesting 18inch as max trace length on a PCB http://www.usb.org/developers/docs/hs_usb_pdg_r1_0.pdf but most USB cables easily going beyond this value).

Do our colleagues here with experience in high-speed signal routing agree? Are USB/DVI/Ethernet cables a trivially easier solution for tens of cm? Intuitively shielding of a cable against EMI and cross-talk seems easier than achieving the same performance with a 4-layer PCB. But then skew control seems easier with PCBs than with twisted pairs. Are we overdoing it by trying to route USB, DVI and Ethernet over 40cm instead of just using cables, even if somewhat untidy inside a production quality enclosure?

How would a top tier design team approach the PCB routing versus cable decision for 40cm signal paths inside an enclosure?

thanks in advance for your comments

Addtional info: To answer the question why I need to take USB/DVI/Ethernet signals as far as 40cm on a PCB, consider a medium size (40cm wide x30cm deep) lab instrument enclosure with a front-panel TFT and multiple back-panel USB/DVI/Ethernet connectors. The MCU/CPU on the main PCB needs to be within 5cm or so of the front-panel TFT (limited by the available flat cable) but the interface connectors need to be at the back of the instrument, >30cm away from the MCU/CPU providing the interface signals. Internal cables are clearly a possible solution. But given the dimensions of the enclosure and internal PCB, routing end-to-end is also possible. The question is, what would be best practise: cables or routing on a large PCB?

\$\endgroup\$
  • \$\begingroup\$ I've never routed such a board so can't tell, but FR4 attenuation at frequencies like Thunderbolt or USB3 uses would be a problem I guess. Cables have much less attenuation. \$\endgroup\$ – peufeu Aug 27 '17 at 21:02
  • \$\begingroup\$ @peufeu Thunderbolt: Don't know the signal characteristics overly well. But: For frequencies of let's say 4 GHz and less, industry standard FR4 should practically be lossless over 40cm – if you design your traces with the right impedance, which might become a challenge, because many standards will assume that traces are short compared to wavelength and hence don't actually specify trace impedance. \$\endgroup\$ – Marcus Müller Aug 27 '17 at 21:05
  • \$\begingroup\$ I mean, server backplanes can easily be full 19" wide and carry PCIe x16. that should be possible. \$\endgroup\$ – Marcus Müller Aug 27 '17 at 21:07
6
\$\begingroup\$

I am by no means an expert in this field (there is a lot going to consider), but...

Are USB/DVI/Ethernet cables a trivially easier solution for tens of cm?

USB, DVI, and Ethernet are all very different, so it's difficult to generalize, but I would say "yes, somewhat". Maybe not for 10-30 cm, but 50 cm+ is definitely getting up there. DVI is definitely the most sensitive; USB 2.0 can run long distances across horrible links, 1G Ethernet uses PAM-5 and is consequently very low bandwidth, but DVI might be unhappy. It might be worth clarifying what specific data rates you are enquiring about.

Intuitively shielding of a cable against EMI and cross-talk seems easier than achieving the same performance with a 4-layer PCB.

Sort of. A cable with a foil shield and drain wire does a pretty good job of protecting the cable from external sources of interference, and proper cable design (twisted pairs with different twist rates) does much to reduce inter-pair crosstalk. When you run traces a long distance on a PCB, they are often quite close to significant sources of noise: planes, power supplies, other high speed digital signals, and due to the geometry of a PCB it can be difficult to protect them. However, you can also embed traces between clean planes, which can result in lanes that perform very well, assuming you have a good stackup.

But then skew control seems easier with PCBs than with twisted pairs.

Yes, skew control is easier, but most high speed protocols design for "consumer-grade" cables are very tolerant of inter-pair skew, although they may be less tolerant of intra-pair skew, the latter of which is dealt with by careful cable design. With USB 2.0 and USB 3.0 SS pairs, there is only one lane, so inter-pair skew doesn't exist. On multilane protocols, there is typically a mechanism by which the receiver can (within limits) compensate for inter-pair skew by "slipping bits" until the lanes are aligned (that is, the receiver looks for synchronization patterns and adjusts a series of single-bit delays to align all the lanes).

For 40cm paths, it depends a great deal on the data rate and how capable your receiver is (i.e. what kind of equalization do you have and how much can you apply?). The loss in FR4 is somewhat linear between 2 and 5 Gbps, so it's typically a matter of doing the maths and figuring out how screwed you are. Simulation tools like Hyperlynx can be very valuable for understanding how traces are effected by PCB structures, connectors, termination, etc.

There are certainly products that aim to fill this gap: Samtec Flyover cable stuff comes to mind, which allows you to route stupid fast signals very long distances, board-to-board (-7 dB insertion loss along 1m @ 8 GHz for example).

If you're really just trying to route USB/DVI/Ethernet along 40 cm of PCB, it might be more appropriate to ask: Why and is it really necessary?

\$\endgroup\$
  • \$\begingroup\$ I think the last paragraph actually deserves most attention: Every signal layout serves a purpose, and it's hard to imagine many devices (short of actual backplanes and signal switches) that would need to transport digital "consumer" signals over such a great length. \$\endgroup\$ – Marcus Müller Aug 27 '17 at 21:27
  • \$\begingroup\$ I have added additional info in the question to clarify the use case \$\endgroup\$ – Eric T Aug 27 '17 at 21:56
2
\$\begingroup\$

The point really is that all of these buses with high speed, but cheap cables, go through relatively great lengths at equalization and deskewing (if parallel). USB3 is significantly more complex than USB2, for example, because a lot of simplifying assumptions on cables can't be made at the higher frequencies.

I'd very much expect shielding and guaranteeing a specific transmission line characteristic being very much harder with connectors and cables than on a PCB, especially a 4-layered one, where you can actually embed microstrip lines between ground planes. Yes, there's surface waves in the PCB substrate, but if you're not making gross mistakes, they will be way less than e.g. radiation off imperfect connectors.

It all comes down to what you need: If you actually just need to bring USB to the other end of your PCB (that is as large already)? Then just route it. Not that much of an additional effort; especially USB2 (even HiSpeed) has become so robust that you really don't need to care a centimeter or three of skew.

Ethernet might be a different beast, but then again, there's definitely extensive equalizing happening, anyway, so I doubt your board layout (and the lengthy trace between logic device and magnetics) will kill you. If you can, compare the (datasheet) effect of having the PHY close to your magnetics and close to your controllers.

DVI: yeah, that sounds like the hardest of these three. But honestly, it's not that many critical lines, and I honestly don't see why your board would perform worse than a cable.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.