I'm designing a PCB featuring a Renesas RZ-A1 microcontroller, and want to check that I'm doing my USB D+ and D- traces correctly.

This application note from Fairchild (alternative link), which is one of the top Google results, says that D+ and D- trace single-ended impedance should be 45 ohms.

Using the EEWeb Microscrip Impedance Calculator, I find that with 1oz/ft^2 copper and a substrate height of 0.08mm, my trace width should be 0.17mm in order to achieve this 45 ohms.

The Fairchild application note also says that the differential characteristic impedance of the D+ and D- lines should be 90 ohms.

Using the EEWeb Edge Coupled Microstrip Impedance Calculator, I find that the spacing between my traces should be 0.098mm in order to achieve this.

Does that look right?

Next part of the question - I understand that series termination resistors are needed on D+ and D-. The Renesas RZ-A1 recommends 22 ohm ones. Does the presence of these resistors change anything in terms of the calculations above? E.g., because the resistors are already providing 22 ohms, should I in fact be aiming for 23 ohm single-ended impedance rather than 45, or something like that?

  • 1
    \$\begingroup\$ USB traces must be 90 Ohms differential. There are a lot of online trace impedance calculators specifically designed for differential traces. Use several of them and compare. They will give very similar answers. The differential impedance will be a bit less than 2x the single-ended impedance. So 90 differential is about the same as 45 single ended. Don't make your traces super narrow unless you have to. 0.17mm seems OK. The differential impedance calculation is not dependent on series resistors. Diff. impedance should be 90 irrespective of the resistors. \$\endgroup\$
    – user57037
    Commented Aug 25, 2016 at 3:47
  • \$\begingroup\$ Closely coupled differential pairs will have a single ended impedance of perhaps 20% higher than half the differential impedance (perhaps a bit more depending on the degree of coupling). As mkeith states, design for 90 ohms differential. The series resistors are to make the total driver impedance 'look' like 90 ohms so it matches the tracks. \$\endgroup\$ Commented Aug 25, 2016 at 7:00
  • 1
    \$\begingroup\$ There must be some misunderstanding. The RZ-A1 has high-speed USB. Usually the HS transceivers have precise self-calibrated 45-ohm impedance, and 22 Ohms should be never used. The 22-ohm series resistors are usually for FS transceivers. \$\endgroup\$ Commented Aug 25, 2016 at 21:30
  • \$\begingroup\$ @AliChen unfortunately the datasheet doesn't appear to specify this. Renesas's own demo board for the RZ-A1 (the RSK+) uses 22 ohm resistors (and some curious decoupling capacitors). My project actually only needs low-speed USB. Any further advice on the situation? \$\endgroup\$
    – beammy
    Commented Aug 26, 2016 at 2:44
  • \$\begingroup\$ Your substrate seems awfully thin - 80um with a 35um copper weight - hmmm. I would expect to see a substrate at least twice this thickness, and even then using 1/2 oz copper. If you are using low speed USB - it probably isn't necessary to use controlled impedance traces anyway \$\endgroup\$
    – N.G. near
    Commented Aug 26, 2016 at 10:09

2 Answers 2


question 1: This doesn't seem right enter image description here

The default Er is 4, but usually the ER for standard FR4 is around 4.6. Although for this calculation you will need the effective Er because the top of the trace is not embedded in FR4.

with Er=4.6, conductor with=0.17mm and dielectric height of 0.08mm the effective Er is 3.2215. but the EEWeb Edge Coupled Microstrip Impedance Calculator not giving me the same values as the polar si800 field solver or the free Saturn PCB toolkit. enter image description here

use the Saturn PCB toolkit it is free and it alco can compensate for the plating trapezoid shape of the traces and other production process variables.

question 2: The trace impedance should be as close as possible to the caracteristic impedance of the cable, the connector and the termination on the receiver end. Any impedance discontinuities will cause reflections and cause degradation to the signal. So keep the trace differential impedance asc lose as possible to 90ohms the single ended impedance is important but not so important because in the cable the signals are transported in a differential pair. the series termination resistors are used for 4 main reasons.

  1. To reduce EMI this is if the product is going to be EC approved.
  2. To absorb near end reflections like the ones caused by the connector.
  3. To control/reduce the signal level in the receiver end because there are maximum drive voltage limits in the HS-USB compliance test.
  4. To crudely improve ESD protection (when the system needs better ESD protection a proper low capacitance clamping device should be used instead)

The only undesired effect is increased slew-rate, but the manufacturer recommendation usually takes this into account.

As a example of using the series resistors to improve compliance please see the following picture. Although the eye diagram perfect, the teat packet failed because it went over the boundaries as signaled by the 3 red dots in the bottom right of the template boundary box. this is because there is some overshooting. The series resistors can be used in this case to reduce the overshooting. enter image description here

the test passes after increasing the series resistor value by 10 ohms.


  • Keep the series termination resistors as close as possible to the pads of the driving device for better absorption of the near end reflections.
  • Avoid running the running the differential pair over a ground plane discontinuity.
  • Keep the differential pair away from any vias, pads or copper in the same layer at least 3 times the inter-pair skew or the dielectric height whichever is the largest.
  • simulate everything
  • if you can reuse a design that is already passing compliance, just do it don't reinvent the wheel.
  • \$\begingroup\$ Nice answer IMO. \$\endgroup\$
    – Rev
    Commented May 2, 2017 at 6:25
  • \$\begingroup\$ Good answer. This should be marked as the answer. \$\endgroup\$
    – mrbean
    Commented Nov 8, 2019 at 22:46

If you follow the Mfg's specs and app notes you will get the best signal integrity. Since the FET inside these class of chips has low RdsOn (10 Ohms) but a wider than desirable tolerance ,a series R must be added but trace impedance should still be 45 Ohms +-10%

Note that the app note uses 42 Ohm at room temp for driver output impedance incl. 29 Ohm.ext. This gives their optimum eye pattern for margin.

Note also that if you scale dielectric thickness up then , so you can uses larger gaps and tracks. **2:1 ratio for track width:FR4 thickness is about right. **

This is because characteristic impedance is due to a fixed ratio if inductance/capacitance ratio or track width to board thickness ratio. The same is true for coax diameter of signal/ground ratio. Distributed Inductance related to aspect ratio of the signal path and capacitance is controlled by the conductor gaps.

enter image description here


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.