# Routing USB2 signals

On this board USB2 signals are routed using smooth lines instead of the usual 45° routing seen on the rest of the board. Does this offer advantages or is this even necessary? A theoretical advantage would be "less reflections", but is this real? Note: I'm not asking about equal length paths, which these aren't.

(One disadvantage I can think of is that not all EDA software let you draw traces this way.)

PS: I saw this on the to-be-announced Arduino Zero board.

• Possible duplicate of electronics.stackexchange.com/questions/74789/… – Mister Mystère May 18 '15 at 14:02
• @MisterMistère: it's not a duplicate. That question turned out to be about equal length paths. – Joris Groosman May 18 '15 at 14:04
• You need to extract information from the answers: the question might have been from a different context, but it was sufficiently general to be answered in a general way and 3 possible causes have been listed. I would place my bet on item 3) of the answer: minimise signal reflections. – Mister Mystère May 18 '15 at 14:05
• @MisterMistère: then my question remains: is it required for USB2? I've never seen it before. – Joris Groosman May 18 '15 at 14:07
• For high speed USB2 perhaps, but I would say it's more good practice than actual requirement. You'd have to look at the USB2 spec. – Mister Mystère May 18 '15 at 14:07

Does this offer advantages or is this even necessary? A theoretical advantage would be "less reflections", but is this real?

It is an advantage. At USB 2.0 rates (480 Mb/s), it's probably not a big advantage, and it certainly isn't necessary. I've seen working designs up above 1 Gb/s using only 45-degree corners.

But it does look pretty, and it doesn't hurt anything.

I would rather see this design made with matched trace lengths and 45-degree corners than round corners but mismatched trace lengths.

I think it's probably trying to ensure a constant characteristic impedance allong the full length of the traces and prevent reflections on the transmission line. As the frequencies of signals increase (and rise times of the outputs of the gates/line drivers get faster) the output cable/traces on a PCB board can be considered to act as transmission lines containing distributed capacitance, inductance and resistance along their length.

If the characteristic impedance ( $Z_0$ = $\sqrt{\dfrac{L}{C}}$ ) along the length of the line changes suddenly, then a reflection of the signal can occur and bounce back to the transmitting device and the reflected pulse interferes with the outgoing pulses messing up the data being transmitted.

If you want to research it some more, look up theory of transmission lines and Time Domain Reflectometry.

Having smooth curves as opposed to 45 and 90% angled corners might be a way to reduce the magnitude of the change of the characteristic impedance, and reduce the reflections and help ensure signal integrity and ensure that data can be transmitted reliably down the line (transmission line, cable, PCB trace) at the required high speed.

• Smooth curves definitely do reduce reflections. If you have 45 or 90 degree angles, a chamfer is usually added to help reduce VSWR on very high frequency designs. To be clear, the smooth curves are best but the difference is likely negligible most cases. – scld May 18 '15 at 17:40

Until 2 weeks ago I would have also said that these make a "better" signal. Yet, tests have shown that it actually doesn't matter in practice (as long as the length is matched):

References (incl. practical measurements):

In my projects I always use the document from Intel, High Speed USB Platform Design Guidelines, when I need to develop something with USB.

This document is published in USB.org site and it says:

• Route high-speed USB signals using a minimum of vias and corners. This reduces signal reflectionsand impedance changes.

• When it becomes necessary to turn 90°, use two 45° turns or an arc instead of making a single 90° turn. This reduces reflections on the signal by minimizing impedance discontinuities.