12

First off:

  • This is for a one-off (or two-off) hobby project, nothing more serious. If this were a commercial design, I would go 4-layer at once (though I wouldn't be designing such a project in the first place).
  • Going 4-layer is acceptable only if TRULY necessary; such boards cost at least twice as much in these quantities, and the 2-layer PCB still costs more than the components combined.
  • The goal is to pass the USB 2.0 signal, mostly unharmed, between two connectors (USB-B to USB-A, both female), nothing more; my PCB does not actually use the signal.

(If these points moves the post into "too narrow" territory, feel free to ignore them :-)

So, the question is: is this possible, with acceptable results? The main goal is, of course, to allow High-Speed (480 Mbit/s) communications.

According to the USB specification, the differential pair should have a differential impedance of 90 ohm, and a to-ground characteristic impedance of 30 ohm. However, USB appears to tolerate a fair bit of abuse; an SMSC app note (PDF) where they discuss 2-layer USB 2.0 PCB layout mentions that the single-ended impedance isn't as critical as the differential, and that a "45 to 80 ohm" range is acceptable.

The board specs are 1 oz copper, with 63 mil FR-4 in between.
According to a few impedance calculators, such as this one (which, unless I misunderstand something, doesn't display the single-ended impedance as well), it appears that 50 mil traces with 10 mil spacing gives ~90 ohm differential and ~80 ohm Z0.
(Those values are from the Saturn PCB Toolkit calculator which is free, but requires download.)

The traces would be on the order of 3 inches long, and likely go in an upside-down U shape to go near the board edges, so that I have space to route everything else (sub-MHz signals only) without breaking the ground plane under the USB traces.

I do of course realize that the entire endeavor is a bit insane; however, again, it's for a hobby board, and it appears to have been done by serious companies as well.
High-speed is really still a bit beyond me, but the rest of the project is simple; I just need to get this signal across the PCB and everything else is a piece of cake.

If you missed it, the main question is: is this possible, with acceptable results?
If there are better 2-layer routing methods (for example, this short article uses coplanar waveguide routing for this purpose), please do tell. I can't find much information (that is both detailed and understandable, but with no details or equation/calculator mentions) about this at all.

djvg
  • 173
  • 8
exscape
  • 1,172
  • 2
  • 12
  • 20
  • If the board does not use the USB signals at all, would it be an option to position the two connectors next to each other? – Anindo Ghosh Nov 08 '12 at 11:27
  • @AnindoGhosh hmm yes, I guess so! I figured having it "in-line" with the cable would be nice, but that is absolutely no requirement, now that you mention it. – exscape Nov 08 '12 at 11:41
  • Then position them close enough to just allow the connectors breathing room as per the USB spec, and put short fat traces between them, preferably of equal length. I would put them at right angles to each other at a corner of the board, such that the whole set-up doesn't interfere with the rest of my PCB. – Anindo Ghosh Nov 08 '12 at 11:48
  • @AnindoGhosh That gives me ~330 mil traces between the pins, or so. They're still 50 mil/10 mil spaced. Something like this: http://i.imgur.com/GVy7j.png (VBUS is the unrouted one, of course.) At least according to some rules of thumb, at 500 ps rise time, this might be below where transmission line effects matter...? – exscape Nov 08 '12 at 12:04
  • 1
    The transmission line effects in this case will be negligible. The only possible concern, if you still want something to worry about, would be that the cumulative length of the two USB cables that you attach to the two ports may exceed the recommended maximum length for USB. – Anindo Ghosh Nov 08 '12 at 12:19
  • Are those two lines correctly routed as per the connector footprints? – Anindo Ghosh Nov 08 '12 at 12:20
  • I'll check again, but I think so. I double-checked when I made the footprints, and the software doesn't allow incorrect routing. – exscape Nov 08 '12 at 12:21
  • let us [continue this discussion in chat](http://chat.stackexchange.com/rooms/6373/discussion-between-anindo-ghosh-and-exscape) – Anindo Ghosh Nov 08 '12 at 12:23

1 Answers1

11

Summarizing comment trail as an answer:

The requirement is for a PCB layout for a pass-through between USB2.0 A and B connectors on a PCB. The rest of the circuit on the PCB does not interact with the USB signal path.

Suggested solution:

By changing the physical arrangement of the two sockets to be close together rather than at opposite sides of the board as originally envisaged, the signal trace length and transmission effect concerns are alleviated.

Further, by setting the two connectors at right angles to each other, at one corner of the board area, the need to leave space between them to allow cables to be plugged in, is addressed: The cables would be connected along different edges of the board and would not touch each other.

This allows simplification of routing as well:

  • The recommendation for equal length signal paths is inherently addressed
  • The arrangement does not interfere with rest of PCB layout, as it is off in a corner
  • With the indicated small trace length, transmission line and antenna effects are negligible for USB 2.0 High-Speed transmissions

Corner layout of USB sockets (as posted by OP).

Concerns that may need addressing:

  • Physical robustness of PCB to cope with stresses of repeated cable insertions - A mounting bolt at the corner between the connectors should address this.
  • Effective total length of USB cable, adding up the A-side and B-side cables, may exceed USB maximum cable length. The very short PCB section would act merely as an extension of the cable.
  • Creative solutions needed for suitably boxing the board with connectors at the corner.
Anindo Ghosh
  • 50,188
  • 8
  • 103
  • 200