The USB IF spec mentions the following for USB 3.0:

enter image description here

This has me scratching my head. In my experience, \$Z_{diff} < 2 Z_0\$ -- typically around 1.6-1.8. So how is it possible to meet both the single and double ended requirements if the single ended requirement needs to be around 50\$\Omega\$ (readily achievable) to get the 90\$\Omega\$ differential impedance?

Some of the resources I've found even explicitly say 50\$\Omega\$, such as this Toradex high speed layout guide (PDF):

enter image description here

And this TI USB 3.0 hub reference design, which uses ~4.5mil trace, 5 mil space on 1oz cu, 3.7mil dielectric thickness also does 50/90:

enter image description here

enter image description here

...but this is straight from the horse's mouth.

Most information I find seems to emphasize the 90\$\Omega\$ requirement more than the 45 ohm requirement. Is it really important to get 45\$\Omega\$ or is 50\$\Omega\$ preferred? Can someone set the record straight for me?


5 Answers 5


In my experience, \$ \text{Z}_{\text{diff}} < 2 \text{Z}_0 \$ -- typically around 1.6-1.8. So how is it possible to meet both the single and double ended requirements if the single ended requirement needs to be around 50Ω (readily achievable) to get the 90Ω differential impedance?

There are two kinds of differential pairs: loosely-coupled differential pairs and tightly-coupled differential pairs. \$ \text{Z}_{\text{diff}} < 2 \text{Z}_0 \$ is only true for a tightly-coupled differential pair. If the difference pair is loosely coupled, the differential pair is essentially two single-ended traces in isolation, thus \$ \text{Z}_{\text{diff}} \approx 2 \text{Z}_0 \$.

Now, read the USB 3 specification again carefully:

The differential characteristic impedance for the SDP pairs is recommended to be 90 Ω +/- 5 Ω. The single-ended characteristic impedance of coaxial Enhanced SuperSpeed signal wire is recommended to be 45 Ω +/- 3 Ω.

Note the keyword: Coaxial! If you're transmitting USB signals in two coaxial cables, obviously, \$ \text{Z}_{\text{diff}} = 2 \text{Z}_0 \$.

Interestingly, the USB 2.0 specification also requires a 45 Ω single-ended and 90 Ω differential impedance, coaxial or not:

High-speed operation supports signaling at 480 Mb/s. To achieve reliable signaling at this rate, the cable is terminated at each end with a resistance from each wire to ground. The value of this resistance (on each wire) is nominally set to 1/2 the specified differential impedance of the cable, or 45 Ω. This presents a differential termination of 90 Ω.

Thus, it's my belief that the USB specifications were originally designed with lower-density circuit boards with loosely-coupled differential pairs in mind. But as routing density has increased, the 45 Ω requirement has not been seriously followed for many years.

Understanding Four Kinds of Impedances

First of all, we need to clarify the concept of characteristic impedance. In a differential pairs, there exists four kinds of characteristic impedance:

  1. Single-ended impedance (\$\text{Z}_{\text{se}}\$): The impedance of the single trace in isolation, when it's excited by a signal between the trace and the ground plane. In single-ended signaling, this is the only kind of impedance.

  2. Odd-mode impedance (\$\text{Z}_{\text{odd}}\$): The impedance of the single trace in a differential pair, when the differential pair as a whole is excited by a differential-mode (out of phase) signal.

  3. Even-mode impedance (\$\text{Z}_{\text{even}}\$): The impedance of the single trace in a differential pair, when the differential pair as a whole is excited by a common-mode (in phase) signal.

  4. Differential impedance (\$\text{Z}_{\text{diff}}\$): The impedance of the entire differential pair as a whole (two traces), when the differential pair as a whole is excited by a differential-mode (out of phase) signal. By definition, it's always \$ 2 \cdot \text{Z}_{\text{odd}} \$.

Loosely-Coupled and Tightly-Coupled Differential Pairs

Using these concepts, let's consider the simplest case: You have two transmission lines far away from each other, and use them to transmit a differential-mode signal. In this case, each line in the differential pair is a single-ended cable in isolation with no interactions with each other. Thus:

$$ \frac{1}{2} \text{Z}_{\text{diff}} = \text{Z}_{\text{odd}}\\ \text{Z}_{\text{odd}} = \text{Z}_{\text{even}} = \text{Z}_{\text{se}} $$

But as the lines in a differential pair is going closer and closer to each other, the electromagnetic field of the two lines starts to interact with each other. And the result is a decrease of its odd-mode impedance relative to its single-ended impedance, and an increase of its even-mode impedance:

$$ \frac{1}{2} \text{Z}_{\text{diff}} = \text{Z}_{\text{odd}} \\ \text{Z}_{\text{odd}} < \text{Z}_{\text{se}} \\ \text{Z}_{\text{even}} > \text{Z}_{\text{se}} $$


To illustrate this, I used a 2D electromagnetic field solver to simulate a differential microstrip line with the following parameters: (1) Metal Thickness of 0.035 mm, (2) Dielectlic Constant of 4.0, (3) Substrate Thickness: 0.1 mm, (4) Trace width: 0.18 mm.

This is representative of a 50 Ω microstrip on the top layer of a 4-layer PCB. The trace separation is varied from 1.8 mm to 0.1 mm. The result is the following, shown as a ratio of the separation distance:

Single-Ended, Odd, and Even-Mode Impedance vs Separation

When the separation distance of the differential pair is 3x the trace width, its single-ended, odd-mode, and even-mode impedance are essentially identical, with a difference about 1 Ω. But as the trace separation continues to decrease, these impedance start to diverge. This is why the differential impedance of a differential pair is often (but not always) slightly lower than two times the single-ended impedance of an individual trace.

This can also be understood as the justification of the "3W rule", a rule of thumb on crosstalk - when there's a 3W separation distance between two traces, crosstalk is negligible. The coupling within a differential pair and crosstalk are essentially the same phenomenon, just utilized for our benefits.

Must Traces in a Differential Pair be as Close to Each Other as Possible?

No. If engineered correctly, both loosely-coupled and tightly-coupled differential pairs work well. And in fact, loosely-coupled differential pairs have several benefits. If routing space is not a problem, a loosely-coupled differential pair is recommended over a tightly-coupled differential pair.

First, it's not always necessary to transmit a differential-mode signal using a tightly-coupled differential pair. If a single-ended transmission lines can already provide satisfactory EMC and signal integrity performance at the same frequency, there is no reason why it cannot be used as one wire of a differential pair. This situation is especially common in laboratory testing, often one uses two separate coaxial cables to carry a single differential pair, since most test instruments are single-ended.

Next, a loosely-coupled differential pair often provides better signal integrity in practice, since it's basically two independent single-ended traces. Meanwhile, a tightly-coupled pair is extremely sensitive to trace separation. Every time you spread or join the differential pair in order to route the signal over a component pad or connector, the odd-mode impedance of a tightly-coupled pair changes significantly. But this has almost no effect to loosely-coupled differential pair.

Finally, a loosely-coupled pair has lower attenuation. As the odd-mode impedance of a tightly-coupled differential pair decreases significantly, to maintain the desired impedance, the width of the trace must also be decreased. This causes an increase of resistive loss and more attenuation.

However, the modern trend is the ever-increasing routing density and miniaturization, thus, loosely-coupled pairs is becoming irrelevant. But if you have this choice, don't forget that it's always an option.


What about EMI/EMC? Shouldn't a differential pair be as close to each other as possible for field cancellation and common-mode rejection?

In theory, yes. But how close is worthwhile? It's a matter of opinion. Multiple authors have argued that there's point of diminishing return due to practical problems.

"Driver Balance" Argument

Dr. Howard Johnson - author of the famed High-Speed Digital Design - A Handbook of Black Magic, argued in the EDN magaine back in 2002 that, a 0.5 mm separation distance in a differential pair is enough for most practical purposes. The EMI/EMC performance would be limited to the skew of differential drivers and there's usually pointless to go beyond that.

Under FCC class B measurement conditions, the differential-mode radiation from a differential-microstrip pair with 0.5-mm separation should theoretically yield a 40-dB radiation improvement at 1 GHz over the radiation you would measure if you implemented the same signal as a single-ended layout. Smaller separations should yield even more improvement. Although that theory sounds appealing, in practice, you will rarely-if ever-achieve as much as a 40-dB improvement in overall radiation because the degree of balance available on the two outputs of your differential transmitter will limit your gains. Unless the outputs balance to better than one part in 100, a common-mode-radiation component of at least 1% of the differential amplitude will emanate from your differential pair anyway. Therefore, even with a differential spacing of zero, you could never improve the total radiation by more than 40 dB.

"Unbalanced Coupling on PCB" Argument

In the book Right the First Time - A Practical Handbook on High-Speed PCB and System Design, the author Lee W. Ritchey presented another interesting argument against routing differential pairs as close to each other as possible.

Ritchey argued that a tightly-coupled pair is helpful in cables and other circuit in free space, where the interference is experienced by both conductors equally. However, the layout on a printed circuit board is planar. The aggressing electromagnetic field will always couple to one side of a differential pair much more than the other side of the pair. In the case of crosstalk experienced by a broadside differential pair, we have two lines, one on the upper layer, another line is on the lower layer. If another unrelated line at the lower layer is driven, it produces 12% crosstalk to the lower line, but 1% crosstalk to the upper line. The differential pair is unbalanced, the interference is not common-mode, and the differential pair fails to reject its interference. The same situation occurs in a coplanar differential pair on the same layer.

Thus, the author argued that the benefit of a tightly-coupled pair is significantly reduced and it's not worthwhile of doing so at the expense of greater routing difficulties.

[Neither side by side routing or above and below routing produces common-mode coupling to a differential pair2

Differential signaling has been credited with other benefits that are inaccurate. One of the most common characteristics as- cribed to differential signaling is that side-by-side routing of the pair of traces in a PCB provides common mode noise rejection. As illustrated in Figure 31.1, this is a false assumption.

It is important to understand that the concept of side-by- side routing cannot guarantee common mode noise rejection in a PCB. Failure to understand this or to depend on it as a way to avoid noise from crosstalk, is one design methodology that results in a flaky system.

Why do people think that side-by-side routing of traces cre- ates common mode noise coupling or noise rejection? It prob- ably stems from the fact that two wires side-by-side in space have this characteristic. This works in free space but not next to a plane because common mode coupling requires the EM field that intercepts each wire be the same strength so that the same size noise signal is induced into each wire. In free space, both wires do experience the same size EM field. In a PCB, this is not possible due to the interaction of the field with the plane. The crosstalk curves in Figures 29.4 and 29.5 can be revisited to see how the strength of the EM field diminishes as it gets farther away from a signal line.

See Also


Single ended impedance is the trace impedance with reference to ground.

Differential Impedance is the impedance between two differential pair signal traces.

So I think both needs to be matched if you want to work at rated high frequency. Also need to be within tolerance range as in USB case it is 15%.

Reference: http://www.ti.com/lit/an/slla414/slla414.pdf (Page # 6)


I think they're talking about two different sets of wires in different generations of the standard.

First sentence refers to SDP, the two Shielded Differential Pairs introduced in USB 3.0 for 5 Gbps throughput. These are usually shielded twisted pairs. Their \$Z_{diff} < 2 Z_o\$.

Second sentence is talking about Enhanced Superspeed, the 10 Gbps signalling introduced with USB 3.1. These can be (high-grade) shielded twisted pairs, but they can also be individual micro-coax wires - one each for the direct and inverted signal of each differential pair. In this latter case because there is little or no mutual coupling between the + and - signals, \$Z_{diff} \approx 2 Z_o\$.

  • \$\begingroup\$ As a caveat: I'm only somewhat confident in this answer. I'm not familiar with USB 3.x. \$\endgroup\$ Jun 16, 2017 at 15:25

My recommendation is to use "loosely-coupled" pairs for this. If you have the space, route 2 SE traces with 45 ohm Z0 using the same path. Keep them 3 or so trace widths apart. This will result in approximately 90 ohm (Zdiff). It is best if you run these traces next to each other (with consistent spacing) and match their lengths. This gets you the benefit of aggressor signals being coupled to both (and therefore largely ignored by the differential receiver).

  • \$\begingroup\$ +1. This is a correct solution. \$\endgroup\$ Mar 19, 2023 at 4:23

SE impedance is controlled by trace width and spacing to the plane mostly.

Diff impedance for far apart pairs is twice the single ended value. As you move the two traces closer, the diff impedance will drop until it's fine.

So choose trace width and prepreg thickness to match the SE impedance, then choose pair spacing to match diff impedance.

A nominal factor of 2 demands quite some gap. I would aim to reach within the specced tolerance. But I also remember some ppl saying ( eg. Rick hartley) that routing the two wires on different areas of the board causes no issues if done right.. so maybe just follow length matching and don't make a diff pair at all.


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.