In the previous article, we covered via design and stub issues. In this article, which is FC33, we will deal with differential pairs. In the beginning of the series (Differential Signals and CMRR), we explained the electrical advantages of differential signals, but in this article, we will explain specific rules for how to route differential pairs at the PCB design implementation level.
Review of Differential Signals—Why Design with Pairs is Necessary
As explained at the beginning of the series, differential signals send signals of opposite phase to the P and N lines, and cancel common-mode noise by taking the difference at the receiving end. To maximize this effect, two conditions are required.
First, the P and N lines must always experience the same noise environment (coupling due to adjacent routing). Second, the signal arrival timing of the P and N lines must match (length matching).
The technology to achieve these two conditions in PCB design is the subject of this article. If these conditions are broken, the theoretical CMRR (Common-Mode Rejection Ratio) will not be achieved, and the noise immunity of the differential signal will be significantly reduced.
Concept of Differential Impedance
The first concept to understand in differential pair design is differential impedance.
Single-ended signals are characterized by the characteristic impedance (usually 50Ω) between the signal line and GND (reference plane) (detailed in FC39).
Differential pairs are characterized by the impedance between the P and N lines (differential impedance, Zdiff). Differential impedance is not simply twice the single-ended impedance, but changes due to electromagnetic coupling between the pairs:
Zdiff ≈ 2 × Z0 × (1 - k)
Z0 is the single-ended impedance of a single trace, and k is the coupling coefficient (0 to 1, larger as coupling becomes stronger).
The required differential impedance varies by standard. USB 2.0 is 90Ω, USB 3.0 is 85–90Ω, CAN (differential) is 120Ω (this is a standard value for termination resistance rather than transmission line characteristic impedance), and Ethernet (100BASE-TX) is 100Ω as a standard value.
Relationship Between Routing Spacing and Coupling
The spacing (gap) between the P and N lines is the most important parameter that determines differential impedance and coupling strength.
Tightly Coupled is an arrangement where the spacing between the P and N lines is set to be equal to or less than the trace width. The coupling coefficient k becomes larger (around 0.3 to 0.5), and the trace width required to obtain the same differential impedance tends to be wider. EMI immunity and noise cancellation effects are maximized, but routing (especially path selection in dense component placement) can become difficult.
Loosely Coupled is an arrangement where the spacing between the P and N lines is set to be larger than the trace width. The coupling coefficient k is small (0.1 or less), and each trace has characteristics close to an independent single-ended line. Routing is easier, but the noise cancellation effect is somewhat weakened.
As a practical guideline, choose tight coupling for high-speed, high-noise environment signals (USB, CAN, etc.), and choose loose coupling when prioritizing the flexibility of routing for relatively low-speed signals. In many FC designs, tight coupling is the default choice.
Specific calculations for trace width and spacing depend on the stack-up (layer spacing, dielectric constant), so use an impedance calculation tool (such as Saturn PCB Toolkit, which will be covered in FC39) to find the combination of trace width and spacing that achieves the target differential impedance (e.g., USB 90Ω, CAN equivalent).
Length Matching
The P and N lines of a differential pair must be made the same length as much as possible.
When a length mismatch (skew) occurs, the signal arrival timing between the P and N lines shifts, causing unintended waveform distortion during differential calculation at the receiving end. This is a concrete implementation issue of the principle explained in the early part of the series (Differential Signals and CMRR), where 'skew prevents the complete cancellation of common-mode noise'.
The guideline for allowable skew is considered as a percentage of the signal's rise time. As a general rule of thumb, it is recommended to keep the timing difference to 1/10 or less of the signal's rise time. For USB 2.0 (rise time of approximately 500ps), the allowable skew is about 50ps, which corresponds to a trace length difference of approximately 7.5mm (calculated from the propagation speed on an FR-4 board).
Length adjustment using serpentine routing (meandering) is a technique to compensate for the length difference that occurred in the actual wiring path by using intentionally meandered wiring patterns. You add meandering to the shorter trace to match the length of the longer trace.
As a design consideration for serpentine routing, if the pitch (folding interval) of the meanders is too narrow, adjacent meander sections may electromagnetically couple, disturbing the original signal characteristics. Regarding the ratio of meander width (amplitude) to trace width, it is generally recommended to ensure a meander gap of at least three times the trace width.
KiCad's differential pair routing tool has a feature that displays the length difference in real-time during routing and automatically inserts meanders within the allowable range. This significantly streamlines the manual length adjustment process.
Intra-pair Skew and Inter-pair Skew
There is a more detailed classification for differential pair length matching.
Intra-pair skew is the length difference between the P and N lines of the same differential pair. The discussion above refers to this intra-pair skew, and it most directly affects the maintenance of CMRR.
Inter-pair skew is the length matching between multiple differential pairs used in an interface (e.g., the TX pair and RX pair of USB 3.0). In many protocols, timing synchronization between pairs is not strictly required, but some high-speed standards (such as PCIe) have specifications for inter-pair skew as well. For common CAN and USB 2.0 used in FC design, management of inter-pair skew is usually unnecessary.
Differential Pair Layer Changes and Vias
The via issues explained last time become more complex with differential pairs.
When a differential pair changes layers, both the P and N lines must move to the same layer at the same time. If only one changes layers first, a length mismatch and a reference plane mismatch occur simultaneously at that moment.
Length matching of the vias themselves also needs to be considered. The parasitic inductance of the vias explained last time may differ slightly between the P-line via and the N-line via (due to manufacturing variations), but at the typical FC design level, this difference is negligible. More important is the overall length matching, including the trace lengths before and after the vias.
The placement of GND stitching vias (explained last time) is particularly important when changing layers for differential pairs. Place GND vias near the layer-change vias so that the return current of each P and N line (or the common-mode and differential-mode current of the entire pair) can return to the appropriate reference plane on the new layer.
Consistency of Differential Pairs and Reference Planes
The principle of return current explained in FC25 is applied more strictly to differential pairs as 'reference plane consistency'.
Differential-mode current (the original signal current flowing in opposite directions on the P and N lines) returns primarily by coupling directly between the P and N lines, so its dependence on a single continuous reference plane is slightly lower than that of single-ended signals.
However, common-mode current (the noise component flowing in the same direction on the P and N lines) depends on the return path through the reference plane, just like single-ended signals. If there is no continuous GND plane directly under the differential pair, the suppression effect of common-mode noise decreases, which can also cause EMI (radiation).
As a practical design guideline, maintaining a single continuous reference plane (usually GND) directly underneath the differential pair throughout the entire routing path is the design that maximizes performance for both differential-mode and common-mode.
Placement of Termination Resistors
Many differential signals require termination resistors to prevent reflections on the transmission line.
CAN bus termination resistors (120Ω, explained earlier in the series) are placed at both ends of the bus. The placement and routing pattern of the termination resistors also affect signal quality. The design that minimizes reflections involves placing the termination resistor at the very end of the bus (closest to the connector) and minimizing the trace length to that point.
For USB, termination resistors (series termination) are often built into the driver side within the standard, so additional termination resistors on the PCB may not be necessary. However, always check the datasheet of the IC being designed for termination requirements.
The positional relationship between the termination resistor and the vias should also be considered. If the termination resistor is placed near the vias from the connector, the aforementioned via stub issue (explained previously) may partially compromise the effectiveness of the termination resistor, so the placement of the termination resistor and the via design around the connector should be considered in an integrated manner.
Differential Pair Design Workflow in KiCad
We will organize the practical flow of differential pair design in actual PCB design tools.
For differential pair definition, register the two related nets (e.g., CAN_H, CAN_L) as a differential pair in the schematic or PCB editor. KiCad has a feature that automatically recognizes pairs by the suffix of the net name (+/-, P/N, etc.).
For trace width and spacing settings, set the trace width and gap that achieve the target differential impedance as design rules, based on the aforementioned impedance calculation results (see FC39).
When using the pair routing tool, use KiCad's differential pair routing mode to route the two traces simultaneously while maintaining the same spacing. This makes it easier to maintain consistency in spacing compared to routing them individually by hand.
For length matching verification, execute the DRC differential pair check function (to confirm if the length difference is within the allowable range) after routing is complete. This is one of the 'items that can be detected by DRC' discussed in the previous and the session before last, and length matching is an area where DRC functions effectively.
Summary
Differential pair design consists of three pillars: differential impedance management (adjustment of trace width and spacing), length matching (skew compensation via serpentine routing), and ensuring the consistency of the reference plane. The choice between tight coupling and loose coupling is a trade-off between noise immunity and routing flexibility. When changing layers, it is important that the P and N lines move together and that a GND stitching via is used to secure a return path for common-mode current. Differential pair length matching is one of the few 'physical validity' verification items that can be checked by DRC, and KiCad's dedicated tools should be actively utilized. In the next session, FC34, we will explain crosstalk—electromagnetic coupling between adjacent traces and its suppression techniques.