4
\$\begingroup\$

Thanks to the help from this community I am much closer to finishing my new design. Right now I am most worried about my USB 2.0 traces, and I want to make sure that I am doing everything right with spacing and what not. I'm using the USB0 port on the NXP LPC4337.

Before I had the USB traces: - grouped together with 6mil spacing except 10mil spacing for D- and D+ like this { USB ID Trace >> 6 mil gap>> USB D+>> 10 mil gap>> USB D->> 6 mil gap>> USB VBUS }

I consulted some colleagues at my school and found that if things were traced this way I could get a lot of noise from VBUS and quite possibly the same with USB ID. I learned that I should isolate D+/D- as much as possible. So I moved the VBUS line onto the bottom layer and far from the D+ D- lines. I'm not sure what I should do with the USB ID line, I've been digging through my data sheet and I can't seem to find anything about running the trace, most of the stuff in it is in regards to control registers and driver development. Any ideas on what I should do for the ID trace?

\$\endgroup\$
  • \$\begingroup\$ Unless you are laying out an OTG device which will switch modes, I wouldn't route the USB ID at all, but if you are it should be a fairly steady-state signal (excepting noise) since usually determined by the inserted connector. 6 mil spacing sounds rather tight and should probably avoided (at least over any distance) unless absolutely required. \$\endgroup\$ – Chris Stratton Mar 17 '13 at 22:54
  • \$\begingroup\$ I'd like the device to be able to implement OTG for future applications but for the project its not necessary. Is it safe to run the ID line parallel to the D-/D+ as long as it is significantly spaced away, say 10 to 15 mil spacing? \$\endgroup\$ – Adam Vadala-Roth Mar 17 '13 at 23:09
  • \$\begingroup\$ @AdamVadala-Roth, Is this a two-layer board or multilayer? What is the height of your D+/D- traces above their ground plane? And what is the length of the traces? \$\endgroup\$ – The Photon Mar 17 '13 at 23:18
  • \$\begingroup\$ @ The Photon, this is a four layer board with the following layer stack profile Top Signal >> Ground Plane >> power plane >> Bottom signal. The USB D+/D- are routed on the top layer (groundplane being beneath them). The traces themselves are about are roughly 2.3 inches long (D-/D+) and are routed as an equal length differential pair spaced 10 mil apart. \$\endgroup\$ – Adam Vadala-Roth Mar 17 '13 at 23:22
  • \$\begingroup\$ What is the height of the first dielectric layer (between D+/D- and ground)? \$\endgroup\$ – The Photon Mar 17 '13 at 23:40
4
\$\begingroup\$

USB ID Trace >> 6 mil gap>> USB D+>> 10 mil gap>> USB D->> 6 mil gap>> USB VBUS

This doesn't sound like a good idea. I'd recommend for other traces, like VBUS and USB_ID, to be further away from D+/D- than D+ and D- are from each other.

Wit 10 mil spacing and a 4-layer board, it's also unlikely that D+/D- are actually working as a closely coupled differential line. This is okay, but you need to think of these traces as two independent single-ended lines that happen to be carrying complementary data. That means it is also a good idea for the potential interfering signals (VBUS, ID) to be further from the high-speed traces than the high-speed traces are from the ground plane. Preferably, if the trace height above the ground plane is h, the other traces should be at least 3 or 4 x h from the high-speed traces.

Note that for USB 2.0, with data rates of 480 Mb/s, your 2-inch (5 cm) traces are approaching the length where transmission line effects begin to matter. It would be good practice to lay them out with the correct width to function as 50-Ohm microstrip lines in your stackup. But again, you're just barely reaching the lengths where this is necessary, so I wouldn't pay extra for your fab shop to guarantee controlled impedance, and if you can't strictly adhere to every best-practice for high speed layout, you will probably still be okay.

I moved the VBUS line onto the bottom layer and far from the D+ D- lines.

This will also be effective for reducing/eliminating interference with the high-speed traces.

\$\endgroup\$
  • \$\begingroup\$ Yeah I moved the VBUS to the bottom far away from D+/D- and I now have the ID traces roughly 80 mil from the D+/D- differential pair. Should that be ok? I know you said I was stretching the USB 2.0 specifications but I can run at the USB 1.0 spec for this particular project. \$\endgroup\$ – Adam Vadala-Roth Mar 18 '13 at 18:11
  • \$\begingroup\$ @AdamVadala-Roth, Not that you're stretching the USB 2.0 specs, but you're right at the low end of the range where you need to start worrying about transmission line issues instead of just making sure the traces connect. \$\endgroup\$ – The Photon Mar 19 '13 at 0:27

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.