I am currently working on the USB hub part for a multiport USB-RS232-converter. The current design is for Terminus Tech's FE 2.1 Hub IC. Regarding the impedance of USB signal traces the layout guidelines state:

DP, DM Differential trace impedance = [DP(45ohm) + DM(45ohm)] = 90 ohm, and do not jump the DP DM signals that cause impedance miss match

To meet those requirements I used some online impedance calculators to estimate the required trace properties for a 2-layer FR4 PCB. However, the results I got are not consistent at all:

  • Hughes Circuits
    • input values
      • trace thickness: 1 oz/ft^2
      • substrate height: 1.6 mm
      • trace width: 1 mm
      • trace spacing: 0.15 mm
      • substrate dielectric 4.5
    • results
      • odd impedance: 45.5 ohms
      • even impedance: 119 ohms
      • common impedance: 59.3 ohms
      • differential impedance: 90.9 ohms
  • Montaro
    • input values
      • trace width: 3.35 mm
      • trace separation: 10 mm
      • trace thickness: 0.03556 mm
      • dielectric thickness: 1.6 mm
      • relative dielectric constant: 4.5
    • results
      • differential impedance: 90.035 ohms
      • single ended impedance: 45.071 ohms
  • All About Circuits
    • input values
      • trace thickness: 1 oz/ft^2
      • substrate height: 1.6 mm
      • trace width: 4.15 mm
      • trace spacing: 14.8 mm
      • substrate dielectric 4.5
    • results
      • odd impedance: 45.0 ohms
      • even impedance: 36.8 ohms
      • common impedance: 18.4 ohms
      • differential impedance: 90.0 ohms
  • Colorado Electronic Product Design
    • input values for single microstrip
      • w: 3.5
      • h: 1.6
      • t: 0.03556
      • epsilon: 4.5
    • result for single microstrip
      • impedance: 45.12 Ohms
    • input values for microstrip pair
      • s: 15
      • h: 1.6
      • Z_0: 45.12 Ohms
    • result for microstrip pair
      • Z_d: 90.23 Ohms
  • EEWeb
    • input values
      • trace thickness: 1 oz/ft^2
      • substrate height: 1.6 mm
      • trace width: 4 mm
      • trace spacing: 5.5 mm
      • substrate dielectric: 4.5
    • results
      • odd impedance: 45.0 ohms
      • even impedance: 38.7 ohms
      • common impedance: 19.4 ohms
      • differential impedance: 90.1 ohms

In addition to those calculation I found some other resources with some sample trace properties:

  • Mikrocontroller.net Forum
    • trace width: 0.22 mm
    • trace distance: 0.13 mm
    • substrate thickness 1.6 mm
    • resulting differential impedance: 100 Ohms
  • IBEX
    • 1.6 mm PCB
    • 1.48 mm FR4 thickness to GND plane
    • 35 um copper trace thickness
    • trace spacing 0.15 mm
    • trace width 1.12 mm
    • resulting differential impedance: 90.184 Ohms

Why do those results differ that much? Since I am a beginner in doing impedance controlled PCB design I do not know which resource to trust. Any hints about dependable trace properties for designing USB on a 2-layer FR4 board are pretty much appreciated.

  • \$\begingroup\$ The top link took me to a single microstrip calculator and not a differential one as per your values that you entered. If you want help fix this. I would also suggest you concentrate on two calculators that have the most disagreement instead of flooding the question with several. \$\endgroup\$
    – Andy aka
    Commented Jan 26, 2018 at 12:50
  • \$\begingroup\$ @Andyaka There is a differential impedance tool on the Hughes Circuits page, but when you select it the URL does not change. Judging by his inputs and outputs he used the correct one. That being said I agree that only posting the two tools that disagree the most would be sufficient. \$\endgroup\$
    – DerStrom8
    Commented Jan 26, 2018 at 12:57
  • 2
    \$\begingroup\$ On EE web you have opted for a trace width of 4mm and a spacing of 5.5 mm yet, on Hughes you have gone for 1mm and 0.15 mm. This doesn't make sense. \$\endgroup\$
    – Andy aka
    Commented Jan 26, 2018 at 13:26
  • 2
    \$\begingroup\$ Not a good way to demonstrate differences because different combinations can produce identical results. \$\endgroup\$
    – Andy aka
    Commented Jan 26, 2018 at 14:35
  • 3
    \$\begingroup\$ You can't make good 90-Ohm traces on a FR-4 1.6 mm two layer PCB unless you allocate HUGE space for channels (and contiguous ground plane). You will have no room for anything else for the USB hub. Forget it. Two layer PCB can be only good for test fixtures, with hundreds of stitching vias along the channel, and nothing around. USB is not the technology for 1.6 mm two layer PCB. Get a 4-layer board. \$\endgroup\$ Commented Jan 27, 2018 at 0:50

3 Answers 3


The reason the values differ so much is because different tools use different formulas to calculate impedance. Some are approximated closer than others, but finding exact impedance is extremely difficult if not impossible. The best tool I've used, and I still use today, is the EEWeb calculator (which you linked to in your post). That one seemed to have the best, most accurate results in my experience. There are also plenty of clones that use the same math as the EEWeb calculator so they will also be just as accurate.

Generally, when designing with controlled impedance as long as you get within +/-20% you will not notice much in the way of reflections and distortion, though of course this depends on frequency and switching speed. However, I try to shoot for about 10% over the target impedance. It's better for the Zd to be higher than the target than for it to be lower. 10% is pretty standard for most designs. In your case I'd shoot for a Zd around 100 ohms (basically 10% higher than your initial target).


The differential impedance depends on many factors including both trace width and trace spacing. For this reason it is possible to have multiple solutions trading off width and spacing. example from eeweb:

thickness=1oz, height=1.6mm, er=4
0.2mm width and 0.02mm spacing = 90.8 ohms differential
1mm width and 0.12mm spacing = 90.4 ohms differential
4mm width and 3mm spacing = 90.4 ohms differential

Choosing the best combination is dependent on several factors including manufacturability (0.02mm spacing is not typically manufacturable on PCBs), current draw(0.2mm is fine for usb but not for high current PoC) and board dimensions.

As for Ale..chenski comment, it is fully possible to make a USB device using a 2 layer 1.6mm fr4 board. It is important that you have an uninterrupted ground plane below the USB traces. This guarantees a consistent impedance and a high frequency return path. With USB 2.0 you can get away with some breaks in the ground plane with stitching capacitors though this should be avoided. USB 3.0+ would be much more susceptible to non-continuous impedance.

Marten's answer would be incorrect as seen here and here. Differential impedance is twice the odd mode impedance. Odd impedance is is the impedance of a single trace when driven in differential mode. The USB standard requires 90 Ohm differential impedance as seen here, that is across both USB_P and USB_N and would equal an odd impedance of 45 Ohm.

Sorry for the edits, can't seem to vote or comment on other answers as a new user...


These calculators ALL use wrong naming for "differential impedance". Actually the "odd impedance" is the correct impedance to look at for the USB requirement of 90 Ohms differential impedance. That's why the numbers Mikrocontroller.net Forum comes closest to the proper track width.


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.