I'm laying out the USB data lines on my board at the moment, and I'm just trying to get an idea of how well off my design is gonna fare. Here are the particulars:

  • 4 layer board (from the top: signal, ground, split power planes, signal)
  • internal copper is 0.5oz, external copper is 1oz
  • prepreg between external foil and core is 7.8 mils thick
  • traces are 10 mil with differential pair spacing at 9.7 mils
  • MCU pin to parallel caps trace length is about 0.23 inches

I plan on having a sealed USB connector in my device's enclosure. The connector I chose has a vertical header arrangement, so I'll have a board that I solder the connector to, and then between that and the main board, there will be a jumper cable.

As far as the differential impedance, based on the above specs, I figure I should be landing somewhere in the 91 - 92 ohms area. Granted, the traces don't stay evenly spaced the whole time since they run through the parallel caps and series resistors before hitting the connector... but I tried the best I could.

Here's a shot of the board layout thus far:

USB data line layout

How does this look? The different in length between the pair of traces is below 5 mils. What I'm concerned about is potentially messing up this whole differential impedance thing... and having the jumper cable between the board and the connector mess things up.

  • \$\begingroup\$ Do you mind sharing what MCU you are using? Many with built in transceivers prefer no external components in line. As long as they are the same length and not too long it should be fine. (I think the Microchip datasheets say less then 19 cm or something absurdly long like that) \$\endgroup\$
    – justing
    Commented Sep 21, 2012 at 19:12
  • 3
    \$\begingroup\$ And how long will the Jumper Cable be? I would guess that will be the weakest link if anything is. \$\endgroup\$
    – justing
    Commented Sep 21, 2012 at 19:14
  • 2
    \$\begingroup\$ You'll probably get away with a lot at the usb low speed / usb full speed rates used by many USB-enabled microcontrollers. If you have something that can do full USB 2.0 high speed, you would likely have to be more careful, though what you have doesn't look bad. \$\endgroup\$ Commented Sep 21, 2012 at 19:43
  • \$\begingroup\$ Jumper cable will be approximately 3 inches long, 28AWG, not shielded. I'm also using an LPC1769. The Embedded Artists prototype board I'm using has the same 33ohm series resistors and 18pF parallel caps that I'm using. \$\endgroup\$ Commented Sep 21, 2012 at 21:14
  • 4
    \$\begingroup\$ It's hard to tell from the drawing but it looks like you are crossing a split in the plane with those two signals and you don't want to do that. USB uses a differential receive, but the signals are still referenced to the plane. Even if they weren't you'd still have common mode noise to worry about. It will probably work like that but it will definitely radiate more. \$\endgroup\$ Commented Sep 21, 2012 at 21:19

1 Answer 1


Assuming you're only using USB-low-speed or full-speed, you should be fine.

Generally, layout considerations only really have to be taken if you're going long distances (many inches), or using USB-2.0. Even then, USB is surprisingly tolerant.

  • USB 1.1 or USB2.0 low/full speed

    • You really don't need to worry. There are (possibly apocraphyal) stories of people running USB2.0 low-speed of 50' of CAT-5 wire. As long as you keep your wire-runs a few inches or less, I wouldn't worry.
    • The fastest edge you will need to worry about in low/full speed applications is 12 Mhz. As such, you're not really approaching the point where making sure your traces/wiring is properly transmission-lined/impedance-controlled is that important, at least as long as your overall uncontrolled-impedance sections are less then, say ~6".
    • As I said, most USB controllers are impressively tolerant of USB devices that are widely out-of-spec. If this is something for production, I would spend the effort to do it properly (there is one guy out there who has a motherboard that throws a hissy-fit if anything connected to it deviates from the spec by a tiny amount), but if it's just a test-board, I'd say just lay it out neatly, and don't worry about it.
  • USB2.0 High-speed.

    • Here layout becomes more important. USB2.0 High-Speed has a maximum edge rate of 480 Mhz. As such, even short traces start to approach the wavelength of the data, and as such proper impedance-control becomes important.
    • Assuming you EDA package has proper impedance-controlled routing options, just set your differential-pair impedance to be ~90Ω, and you should be fine. Be careful to make sure you have a contiguous ground-plane, though
  • USB3.0

    • So you hate yourself?
  • \$\begingroup\$ Honestly, there is the potential that some guys I know might want this. I don't want to rule out selling it so designing it right, if it's not going to require me to go to ridiculous lengths, is big for me. I only plan on supporting USB 2.0 Full-speed, though. Would I be better off having the board that the connector solders into plug directly into the mainboard and run traces all the way to the edge of the main board? At least that way I could control impedance better, potentially, than I'd be able to with a jumper cable. \$\endgroup\$ Commented Sep 22, 2012 at 1:38

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.