Impedance Matching for USB Interfaces in PCBs

Key Takeaways

• The differential characteristic impedance of the USB 2.0 and USB 3.x interface must equal 90Ω ± 15 % tolerance.

• Geometrical parameters such as trace width, height above the reference plane, distance between traces, and trace length can be adjusted to achieve the desired standard impedance matching for USB interfaces.

• The impact of impedance mismatching for USB interfaces both for 2.0 and more so for 3.x include signal reflections, signal loss, crosstalk, and noise.

Modern electronics utilize USB interfaces for high-speed data transfer

Impedance matching for USBs is essential to obtain the desired performance from peripheral devices in consumer, industrial, and automotive applications. The USB interface is based on differential pair signaling, and standard values for the differential characteristic impedance are subjective to the USB generation. We will discuss impedance matching for the USB 2.0 and USB 3.x interface in this article. 

The Effect of Impedance Mismatches in USB Interfaces

Generally, USB interfaces allow signal or data transfer between a device and another peripheral. Impedance matching for USB interfaces in PCBs is a significant factor in controlling signal degradation. If the impedance standards are not met while routing the traces of the USB interface on the PCB, the receiving end signal is distorted. Impedance mismatches in USB interfaces can have negative effects on signal integrity. Signal degradation issues can result in output errors, which can be costly.

Standard Impedance Matching for USB Interfaces in PCBs

Schematic of USB 2.0 interface

USB 2.0 utilizes the differential pair of signals D+ and D- along with the VBUS and GND, as shown in the figure below. There are two pairs of differential traces in USB 3. X generation. The table below gives the standard differential characteristic impedance values for USB 2.0 and USB 3.0.

Standard impedance values of USB 2.0 and USB 3. X interface

The operating frequency of USB 2.0 can be categorized as given in the table below.

Frequency scale of USB 2.0 interface

Even if the frequency scale differs, the impedance values for all USB 2.0 speeds are the same.

Single-Ended and Differential Characteristic Impedance Influences Impedance Matching for USB Interfaces

A USB 2.0 interface differential pair can be routed on external or internal PCB layers. Let's consider a USB interface differential pair routed on the external PCB layer, as shown in the figure below. 

Schematic of USB 2.0 interface traces

In this case, the single-ended characteristic impedance and differential characteristic impedance can be given by the following micro-strip impedance equations.

Note that Z₀ is the single-ended characteristic impedance, Z_d is the differential characteristic impedance, d is the distance between the D+ and D- trace, w is the width of trace, t is the thickness of trace, h is the thickness of the dielectric, and ∈_r is the relative dielectric constant.

It is clear from the equations that the single-ended characteristic impedance of the transmission line influences the differential characteristic impedance. According to USB standards, the single-ended characteristic impedance must be within 45Ω ± 15 % and is mostly dependent on the trace width, height, and dielectric constant of the PCB material.

As per the standards, equations (2) and (3) must equal 90Ω ± 15 % tolerance. The ratio d/h is very important in the design of the USB interface, as the length of the differential traces (D+ and D-) and the distance between them control the differential characteristic impedance value.   

Coupling Between Differential Pairs and Impedance Matching in USBs

The distance between the D+ and D- traces of the USB interface affects coupling. As the distance between the traces decreases, the coupling between them grows and vice versa. The higher the coupling, the lower the differential characteristic impedance. The geometrical parameters such as trace width, height above the reference plane, the distance between the traces, and trace length are adjusted to achieve the desired standard impedance matching for USB interfaces.

USB 3.x Guidelines

With the advent of USB 3.x, the design complexity increases significantly due to higher data rates and additional differential pairs required for SuperSpeed data transfer. Unlike USB 2.0, USB 3.x employs separate differential pairs for SuperSpeed data (commonly referred to as TX/RX pairs). These additional pairs are used alongside the traditional USB 2.0 signals to achieve data rates up to 5 Gbps (USB 3.0) and beyond for later revisions. USB 3.x connectors include extra pins to accommodate the SuperSpeed pairs. At higher data rates, even minor mismatches in trace lengths can result in significant skew between differential pairs, necessitating more attention to impedance matching for USB 3.x.

USB 2.0 vs 3.x Pinouts

SuperSpeed in USB 3.x

SuperSpeed is the high data transfer mode introduced with USB 3.0 and later versions. The SuperSpeed Transmitter is the circuit component responsible for sending high-speed data from the host device. It operates using a dedicated differential pair designed to deliver high-frequency signals with controlled impedance. By converting digital data into these high-speed analog signals, the SSTX ensures that data is transmitted quickly and accurately, minimizing signal degradation and reflections. Complementing the transmitter, the SuperSpeed Receiver captures the high-speed data sent over the dedicated differential pair. The SSRX should be engineered with similar impedance control measures to effectively receive and convert the incoming signals back into digital data.

In USB 3.x, a dual-bus architecture is implemented. The legacy USB 2.0 D+/D– lines handle device enumeration, control signaling, and fallback operation, while the dedicated SuperSpeed TX/RX pairs manage full-duplex high-speed data transmission. Although both interfaces remain active simultaneously, high-speed data transfer occurs exclusively over the SuperSpeed lanes.

Challenges in USB 3.x Design

The need to route multiple differential pairs—each with their own impedance requirements—means that PCB layout must be optimized not only for individual trace characteristics but also for minimizing interference between adjacent pairs. Techniques such as controlled dielectric spacing and careful via placement are essential.

Summary of Challenges in USB 3.x Design

Differences Between USB 2.0 and USB 3.x

USB 2.0 involves a single differential pair for data transfer with less stringent length matching and routing requirements, whereas USB 3.x requires multiple differential pairs for SuperSpeed communication, requiring tighter control over trace geometry, spacing, and length matching.

Signal Integrity and Routing

In USB 2.0, signal integrity issues are managed with standard microstrip routing techniques, and the impact of minor mismatches is relatively moderate. In USB 3.x, high-frequency signaling requires that designers minimize impedance discontinuities, and control crosstalk more rigorously. The extra differential pairs must be routed with extra attention to spacing and coupling, often requiring additional layers or dedicated routing channels.

Impedance Matching for USB 3.x

While USB 2.0 and USB 3.x both require a differential impedance of 90Ω ±15%, meeting this specification in USB 3.x designs is significantly more demanding due to increased data rates (5 Gbps for USB 3.0, 10 Gbps for USB 3.1, and 20 Gbps for USB 3.2 Gen 2x2). At these frequencies, transmission lines are highly sensitive to discontinuities and impedance variations introduced by physical design elements. Layout guidelines for USB 3.x differential pairs include:

• Trace width and spacing: Must be tightly controlled according to the PCB stackup to maintain the 90Ω target. Use field solver-driven impedance calculators to model variations.
  

• Skew control: Inter-pair skew should be less than 15 ps to avoid timing mismatches; this translates to a trace length mismatch of less than ~100 mils on FR-4 (assuming ~150 ps/in propagation delay).
  

• Via design: Back-drilled vias or blind/buried vias are recommended to reduce stub lengths; stubs longer than 150 mils can cause significant reflection at USB 3.x frequencies.
  

• Return path integrity: Ground reference planes must be continuous beneath differential pairs. Avoid split planes or gaps, which increase loop inductance and degrade impedance control.
  

• Connector and component models: Use S-parameter or IBIS-AMI models to simulate signal integrity across connectors, ESD protection circuits, and other inline components.
  

Designers should also follow the USB-IF electrical compliance guidelines, which include eye diagram templates, insertion loss budgets, and jitter tolerance limits for SuperSpeed signaling. Full-channel simulation using tools like Sigrity is recommended to validate signal quality prior to prototyping.