At 112G PAM4 the signal has a 28 GHz Nyquist frequency, and PCB insertion loss stops being a detail and becomes the link budget. Here is what actually moves the number, and which of those levers a fabricator can control.

Why 112G Changes the Rules
A 112G PAM4 lane runs at 56 GBd, so the fundamental frequency is 28 GHz and the energy that matters extends past 40 GHz. At those frequencies the copper trace is no longer a wire with negligible loss; it is a transmission line where dielectric absorption, copper surface roughness and every impedance discontinuity subtract from the eye.
The practical consequence is a loss budget. A typical 112G link can afford roughly 30 to 35 dB of channel loss end to end, and the PCB usually consumes half of it. On a 10-inch trace that works out to about 1.5 to 1.8 dB per inch, which is why material choice stops being a cost decision and becomes a feasibility decision.
What the Number Is Made Of
Insertion loss in a PCB trace has four contributors, and they do not scale the same way with frequency.
| Contributor | Behaviour | Who controls it |
|---|---|---|
| Dielectric loss | Rises roughly linearly with frequency; set by Df | Material selection |
| Conductor loss | Rises with the square root of frequency through skin effect | Copper weight, trace width |
| Surface roughness | Adds to conductor loss at high frequency | Copper foil type |
| Discontinuities | Via stubs, layer transitions, connectors | Stackup and back-drill |
At 28 GHz, dielectric loss dominates on long traces. On short traces inside a package escape, the discontinuities dominate instead. That is why a board can pass on a 10-inch coupon and fail in the real channel: the coupon measured the material, not the vias.
Lever One: Dissipation Factor
Df is the single largest lever, and the gap between grades is wider than most people expect.
| Material class | Df at 10 GHz | Loss on a 6-inch trace at 28 GHz |
|---|---|---|
| Standard FR-4 | 0.020 | roughly 15–18 dB |
| Mid-loss | 0.008–0.010 | roughly 9–11 dB |
| Low-loss | 0.004–0.006 | roughly 6–7 dB |
| Ultra-low-loss | 0.001–0.002 | roughly 4–5.5 dB |
On a long backplane run, standard FR-4 simply cannot open a 112G eye. On a short accelerator-card trace it can, which is why hybrid stackups exist: ultra-low-loss on the layers that carry the high-speed pairs, high-Tg FR-4 on the power and ground layers where loss does not matter. Paying ultra-low-loss prices for twenty layers of laminate is not necessary and does not improve the link.
Lever Two: Copper Roughness
At 28 GHz the skin depth in copper is under half a micron. The signal is travelling in a layer thinner than the surface profile of ordinary copper foil, so the current path follows the peaks and valleys and the effective path length grows. This is why the same laminate can measure very differently with standard foil and with HVLP foil.
Surface roughness is usually quoted as Rz. Moving from a conventional foil at Rz 4–5 µm to a very-low-profile foil at Rz 1.5–2 µm typically recovers 1 to 2 dB on a 10-inch 28 GHz channel. It also matters which side of the laminate the foil is on, because the copper on the outer layer and the copper on the inner layer are not the same foil.
Lever Three: Via Stub and Back-Drilling
A through-via on a 3 mm board leaves an unused barrel below the layer where the signal enters. That stub is an open-circuited transmission line, and at a quarter wavelength it resonates. On a 3 mm board the first resonance lands close to 12–14 GHz, squarely inside the 112G band.
Back-drilling removes the stub, and the residual length has to be short enough that the resonance moves above the band of interest. In practice the target is 4 mil or less, with depth tolerance of about ±2 mil. A 10 mil stub is enough to ruin return loss even when the insertion loss looks acceptable on a sweep, because the damage shows up as a notch rather than a slope.
Lever Four: Dk Uniformity and Glass Weave
Dk sets the impedance and the propagation delay, so variation in Dk across the board becomes skew between lanes. Woven glass bundles and resin-rich areas have different Dk, and on a differential pair routed parallel to the weave the two traces can see different effective Dk. The result is intra-pair skew that no amount of length matching fixes.
Spread-glass or flat-glass laminates reduce the effect. Routing the pair at an angle to the weave helps. Neither is a manufacturing fix; both are design decisions, but the fabricator is the one who can tell you which laminate in stock actually has the flat weave.
What a Coupon Actually Tells You
Most insertion-loss data comes from a test coupon, not the product board. A coupon is useful if it matches the product in three things: the same stackup, the same trace width and the same via structure. A coupon with no vias, built on a different stackup, measures the laminate and nothing else.
We measure impedance by TDR and, where the customer supplies a pattern, insertion loss by VNA on coupons that replicate the product stackup including the back-drilled vias. The results travel with the panel lot rather than being reported once at qualification.
Practical Rules
| Parameter | Target for 112G PAM4 |
|---|---|
| Df at 10 GHz | ≤ 0.004 on high-speed layers |
| Copper foil | HVLP, Rz ≤ 2 µm |
| Residual stub | ≤ 4 mil after back-drill |
| Impedance tolerance | ±7% differential |
| Intra-pair skew | ≤ 5 mil, with weave-aware routing |
| Loss budget for PCB | ≤ 0.5 dB per inch at 28 GHz |
None of these is exotic on its own. The difficulty is holding all of them at once on a 20-layer board where the power planes want heavy copper and the high-speed layers want thin, smooth foil.
What to Send for a Stackup Review
The Gerber, the stackup drawing with layer assignment, the impedance targets per net class, and the loss or eye budget the channel has to meet. From those four we can say whether the stackup will make the number, and if not, which lever moves it cheapest: material, foil, back-drill depth or layer assignment.
Related: 20-layer 4-stage HDI PCB for AI accelerator cards and 24-layer AI server mainboard PCB.
Related reading
- High-Speed PCB Design: Signal Integrity & Impedance Control
- Antenna Switching PCB Design: Diversity and MIMO Path Selection with Minimal Insertion Los
- RF Combiner Board PCB Design: High-Power Combining with Minimal Insertion Loss and Isolati
- Robot High-Speed Backplane PCB: PCIe and Ethernet Bus Design and Manufacturing
- High-speed PCB manufacturing
- UBB GPU baseboard PCBA