0
\$\begingroup\$

I wanted to make a device that has a USB A and a USB C connector on apposing sides of the PCB, similar to the attached image. dual usb memory stick These USB connectors would be connected to the same USB port, the MCU I am using has only one USB port. The connection type would be USB 1.1 full speed. One of the connections can be made under the critical length, the other one I would have to run matched impedance controlled traces to. I am just wondering if I have to worry about the traces for the connection that is not being used, acting as a capacitor or inductor. Is there anything else I have to worry about?

\$\endgroup\$
4
  • \$\begingroup\$ "One of the connections can be made under the critical length, the other one I would have to run matched impedance controlled traces to." You do realize that the data lines are a differential pair, and should be routed as such? (In parallell, equal length) Regarding impedance matching, I wouldn't worry about it for full speed USB if the traces are less than like 200 mm or so. \$\endgroup\$
    – Klas-Kenny
    May 13, 2022 at 6:03
  • \$\begingroup\$ USB 1.1 Full speed does not care about HF impedance much, especially when the traces are not very long. Remember, we are talking about 6MHz here (IIRC). \$\endgroup\$
    – Turbo J
    May 13, 2022 at 6:50
  • \$\begingroup\$ The question is, why do you want to do that? USB connections can't be split into two connectors so it makes no sense to do that, unless you can mechanically enforce that only one connector can be used at one given time. Even having just an extra cable connected in addition to the one you want to use will cause problems. Will the MCU be a USB host or device? It might be simpler to just use an USB mux to switch between connectors. \$\endgroup\$
    – Justme
    May 13, 2022 at 8:49
  • \$\begingroup\$ @Klas-Kenny it's not true that diff pairs must be routed together. Length matches yes, but routing in parallel is a deliberate choice and nothing prevents perfect functionality and EMC even if the traces are far apart or even on different layers. Most return current anyway flows in the reference planes. \$\endgroup\$
    – tobalt
    May 13, 2022 at 9:51

1 Answer 1

1
\$\begingroup\$

USB Full Speed is simply symmetrical* 12MHz LVCMOS logic levels. It's very far from a signal quality concern; fast enough to need proper cables, low enough voltage to need shielding, but at the PCB level, trace width, and length (up to a generous limit) are largely irrelevant.

*Except when they're not; the start and stop symbols are asymmetrical (both lines moving in the same direction, not complementary). Which is another reason why USB is difficult to filter noise off of, and why contiguous shields are mandatory.

You will have no problems, with a board sized as pictured.

However, if you're expecting performance up at High Speed, these concerns are more justified. Still not a problem on a board that size, I think (the stub length of either connector will be, what, a cm or two, at most?). Super Speed will probably not work with such stubs. (But, since SS isn't supported by USB-A, it would be quite strange to route those pairs to a connector that doesn't even have pins for them. :) )

The deciding factor is if a stub length or mismatch length is a substantial fraction of a bit-time: for High Speed, this is in the low ~cm. Trace mismatch isn't extreme in most situations: the usual worst case is thin traces on a thick substrate (i.e. 2-layer board): the differential impedance is in the 150-200 ohm range, when 90 or so is required; so, it's only a 2:1 mismatch, not at all extreme. Mismatch becomes proportionally more significant when it's worse -- but it's hard to even conceive of a situation with, like, 600 ohm twin lead, on a PCB with ground plane (good luck with that?!), and even then that's a ~5x mismatch so only 5x more sensitive, or a problem for "low ~cm" / 5 -- say, >3mm worth.

In general, when mismatch is some factor, the critical length is shorter by the same factor; for example, we can apply this to the layout of switching converters, where the impedance might be a mere 5 ohms ballpark (say for a 5V 1A converter). Relative to say ~100 ohm traces, that's a mismatch of 20x. If the converter's maximum harmonic frequency is ~200MHz (typical for modern switching regulators), the critical length is a wavelength of ~4GHz. So, a cm or so -- hence why we minimize layout area of these circuits. The same logic applies to most digital communications, and so we minimize the layout area for them as well, with the scale factor (for what counts as "minimized") given thusly.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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