0
\$\begingroup\$

The USB ESD protection component USBLC6-2SC6 seems to be very popular (?). However, its pinout seems not ideal:

  • The USB differential pair should be routed close to each other, but the pinout of USBLC6-2SC6 requires fanning out the differential pair and wedging VBUS and GND in between.
  • The USB differential pair should run over an uninterrupted ground plane, which makes the routing of VBUS a bit weird on 2-layer PCBs, and many designers end up splitting the ground plane.

Why is the pinout of USBLC6-2SC6 so weird (with D+ and D- not on neighboring pins)? Are there better alternative parts without disadvantages?

pinout: IO1, GND, IO2 on one side, IO1, VBUS, IO2 on the other side

\$\endgroup\$
1
  • \$\begingroup\$ Guessing, if this chip was just for over / under voltage protection, then it does sound more convenient to pick a chip where the USB pins were adjacent. But it might be that ESD requirements made it difficult to pass tests w/o routing ground between the IO pins. \$\endgroup\$
    – st2000
    Commented Jul 1, 2023 at 12:44

1 Answer 1

Reset to default
2
\$\begingroup\$

Sure, it's not ideal, at least not for two-layer PCB, but on the other hand, it's good enough and two-layer PCB is not ideal for USB anyway.

The point of the differential data pair is not to strictly wire the two wires as a wire pair that are close together; the point is to have the defined differential impedance, and for that, they do not need to be wired as a pair close together, as 90 ohm differential pair is the same as having two separate 45 ohm single ended wires.

And for standard thickness 2-layer PCBs, you can't anyway properly define a 90-ohm differential pair, so if the impedance matching is off anyway, it's not a professionally designed product but sounds more like a one-off hobby project, so it makes no sense to be pedantic about ESD protector pinout, as you can just decide not to put any extra ESD protection.

And second thing is that when you use a proper 4-layer PCB, then the wires can go as differential pair over non-broken ground plane, separate for a few millimters at the ESD device, and the GND and VBUS can simply be vias to GND and supply planes.

The part is very symmetric for data lines and is ideal for being in-line, and allows good protection without stubs. This is very hard to beat.

\$\endgroup\$
6
  • \$\begingroup\$ Regarding "properly define": What's the problem with 90-ohm differential impedance on standard 2-layer PCBs? I can calculate the appropriate trace width and spacing. If the calculation is inexact, I can make measurements and iterate. Right? \$\endgroup\$
    – root
    Commented Jul 1, 2023 at 13:39
  • \$\begingroup\$ @Root You can calculate anything and get some results. What you don't know is are these results even valid. What numbers do you get, are the numbers sensible, and does the used formula used support those numbers? \$\endgroup\$
    – Justme
    Commented Jul 1, 2023 at 13:44
  • \$\begingroup\$ Several calculated combinations of trace width and spacing are listed here, but that's not the point. If some calculation is wrong, I can make real-world measurements and iteratively adjust the trace width and spacing until the differential impedance is 90 ohms, right? I don't understand what you mean by "can't anyway properly define". \$\endgroup\$
    – root
    Commented Jul 1, 2023 at 14:02
  • 2
    \$\begingroup\$ @root OK, as a simple example, a certain tool I used specifies that both S/H ratio and W/H ratio must be between 0.1 and 3.0 to be reasonable. As H is 63 mils, even if you set S to 6.3 mils, each data wire must be 47 mils, or 1.19mm wide. Assuming your PCB can even be manufactured down to 6.3 mils spacing, you are still living at the extreme end of S/H ratio being 0.1, and even that makes a total of 2.5mm width for USB data, which is completely absurd width for data wiring, so in practice you will end up with wider gap and wider tracks. USB2 on 1.6mm is extremely impractical if even possible. \$\endgroup\$
    – Justme
    Commented Jul 1, 2023 at 15:10
  • 1
    \$\begingroup\$ @root It really depends what other thins are different. For example, even if differential impedance of two scenarios is identical, it means the two scenarios have different single-ended impedance for each wire of the pair. It should also be in some sensible range suitable for USB. So not only differential impedance is important as it is a combination of one wire getting coupled with both the other wire and ground, so they have also single-ended and common-mode impedances. \$\endgroup\$
    – Justme
    Commented Jul 3, 2023 at 5:32

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