1
\$\begingroup\$

I need your advice regarding the USB 2.0 signals routing. When I reach the USB connectors, the data lines (D+ and D-) have to be swapped. I have two options there: 1) swap the lines using vias and go from top to bottom layer for a short, 2) make a loop around the connector, like in the following picture.USB data lines routing

What is your suggestion, what is better option in therms of signal integrity ? I just wonder if this loop emphasizes antenna effect, but maybe the option with vias is worse.

P.S. Just to avoid confusion,bellow the top layer, there is a solid GND plane, so this split plane is power plane (layer 3), not the GND plane.

Thank you for your time, Igor

| improve this question | |
\$\endgroup\$
  • 1
    \$\begingroup\$ I can't think how a few mm of extra traces could be worse than vias. Maybe I would just fix the distance difference on the last stretch of traces (where they match the connector pitch). I'd make them the connector pitch just before touching the pads. \$\endgroup\$ – Wesley Lee Feb 3 '18 at 20:07
  • \$\begingroup\$ Am I correct that you have a four layer stack up of signal (top), ground, power, and signal (bottom)? Yeah, I agree with @WesleyLee that via and crossing on a different layer would probably introduce significantly more impedance disruption of the differential pair than looping it around the connector as you show. \$\endgroup\$ – TimB Feb 3 '18 at 20:22
  • \$\begingroup\$ Yes, you are correct about four layer stack up. Thank you for observation. \$\endgroup\$ – IgorEkis Feb 3 '18 at 20:35
  • 1
    \$\begingroup\$ It looks like you have your USB lines crossing a slot in the ground or power plane. Don't do that without bypass capacitors providing an AC return path. \$\endgroup\$ – akohlsmith Feb 4 '18 at 5:25
0
\$\begingroup\$

Short tracks are always nice, but differential pair and length matching is more important.

With vias you will change reference plane and you will have to put extra caps to connect reference planes.

Loop is just fine, the extra EMI noise will be rejected because it will be common on both signals.

Impedance in pair must be as matched as possible, near connector the gap is much bigger than the rest and there is no length matching.

Its a nice practice to make it so the signals will travel together. On AD its fairly easy.

USB 2 is slow, it will work just fine in your pic.

| improve this answer | |
\$\endgroup\$
0
\$\begingroup\$

For 480MHz (HS) USB, you need to length match the traces to within 150mils, but otherwise going the long way around is fine.

It's hard to tell what the amber area is, but you should avoid crossing planes if possible.

The full layout guideline for USB 2.0 is here: http://www.usb.org/developers/docs/hs_usb_pdg_r1_0.pdf

| improve this answer | |
\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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