3

I found that it's always recommended to use at least 4 layers for high speed routing, but there are still some projects which uses only 2 layers for USB high speed.

I'm just a hobbyist, I cannot effort for high cost board. Can you explain me why some project like this one (http://www.pavouk.org/hw/audiosystem20/en_at32uc3a3256usbi2s.html) or this one (http://dangerousprototypes.com/docs/FT2232_breakout_board) can use only 2 layers board for USB high speed. How can I do like them? Is there any further materials about this technique?

Thank you very much.

dazzlingvit
  • 31
  • 3
  • Multilayer boards are really required in cases where high-speed signalling is required over USB (i.e. USB 3.0). However, two-layer boards are ok for lower speed connections. – DerStrom8 May 18 '16 at 16:37
  • Your best bet is to keep the traces between the USB connector and the USB IC as short and direct as possible by putting the IC immediately at the connector, and perhaps give yourself a spot for series terminating resistors you can experiment with if you find it doesn't just work. Be careful of power routing and bypassing too. If you are making a one-off for personal use, your requirements may be lower - it doesn't have to work with everything, just for you. What four layers does is give you layout flexibility, low power/ground impedance, and a greater variety of possible trace impedance. – Chris Stratton May 18 '16 at 16:40
  • 1) How do you know they work? And how well they actually work? It's much easier to get it right on the first pass with a 4+ layer board. 2) The distances are short and they're getting away with it. – scld May 18 '16 at 16:58
  • You can do USB ona 2 layer board if you use coplanar waveguide, which can be done without a reference on a separate layer. – Peter Smith May 18 '16 at 17:03
  • @scld: Actually I don't know. I just guess because these are popular hobbyist sites. – dazzlingvit May 19 '16 at 12:04

2 Answers2

2

USB has quite a bit of margin built in to account for imperfect connectors, circuit board routing, cables, etc. Best case scenario, the layout and routing in your design will be implemented as closely as possible to the standard to ensure that the portion of the margin your implementation eats up is small.

In the case of the Dangerous Prototypes PCB, the 2-layer based routing may not be ideal, however with the provided USB cable, there's likely still enough margin left. It is possible, however, that if you increased the length of the cable, or added more hubs into the mix, the link may not be as reliable. This is OK for a development board, however, for a product requiring a high level of robustness, sticking closer to an implementation that can achieve the USB spec would justify an increased cost.

The USB standard specifies differential impedance between the data pair (D+ and D-), as well as the impedance of D+ and D- to GND. Differential impedance is dependent on trace width and spacing between the pair. Proper impedance to GND would be most achievable with a reference ground plane on the layer directly adjacent the surface layer D+ and D- are routed on, which would make a 4+ layer board a better option. Note that the insulating layer thicknesses and dielectric properties between the routing layers also play a role, so simply moving to any 4-layer board wouldn't necessarily get you within spec.

Ultimately if you are a hobbyist looking to make a device that would normally operate in a more controlled environment, Chris Stratton's response is very reasonable:

  • Include some series R on the D+ / D- traces (initially populated with jumpers) that can be experimented with in case of communication issues.
  • Locate the IC and connector close to keep the D+ / D- pair's routing short.
  • Match the length of the D+ / D- traces as closely as possible.
  • Route other traces as far away from the pair as possible.

There's also a similar question asked here: 2-layer USB 2.0 High-Speed routing

Community
  • 1
dochex
  • 21
  • 2
0

Choose a thin dielectric between layer one and ground to simplify attaining accurate impedance for critical lines, especially for the USB differential pairs. Make the boards as thin as practical. http://ww1.microchip.com/downloads/en/AppNotes/an262.pdf page 6 Stack up

user150261
  • 1