Signal Integrity and High Speed Digital High Speed PCB Design Informational

How do I select the right PCB material for a 25 Gbps or 56 Gbps serial link?

Q: Can I mix materials in the same stackup?

Yes. Hybrid stackups are common and cost-effective. Signal layers (high-speed SerDes): use low-loss laminate (Megtron 6). Power/ground layers: use standard FR-4. Consideration: the different Dk values between layers must be accounted for in the impedance design. The lamination compatibility (CTE, glass transition temperature) must be verified with the PCB fabricator.

Q: How important is copper roughness?

At 5 GHz: roughness contributes approximately 10% of the total conductor loss. At 25 GHz: roughness contributes 20-40% of the total conductor loss. Using HVLP copper (Rz < 2 μm) instead of standard HTE (Rz 5 μm): saves approximately 10-20% of the total trace loss at 25 GHz. For 56+ Gbps designs: HVLP copper is mandatory (the roughness loss is too significant to ignore).

Q: How do I verify the PCB material performance after fabrication?

Request test coupons on the production panel. Measure insertion loss vs frequency using a VNA with appropriate fixtures (PCB launches). Compare the measured loss to the simulation (which uses the specified Dk and Df). The measured loss should agree within ±10% of the simulation. If significant discrepancy: investigate the material Dk/Df (request material test reports from the fabricator), the copper roughness (SEM cross-section), and the impedance (TDR measurement on the coupon).

How do I select the right PCB material for a 25 Gbps or 56 Gbps serial link? The PCB material (laminate) determines the dielectric loss, copper roughness loss, and impedance stability, and becomes the dominant loss contributor at high data rates: (1) Key material parameters: Dk (dielectric constant): determines the signal propagation speed and trace impedance. Standard FR-4: Dk = 4.0-4.5 at 1 GHz. Low-loss laminates: Dk = 3.0-3.7. Lower Dk allows wider traces for the same impedance (better loss). Df (dissipation factor / loss tangent): the primary measure of dielectric loss. Loss (dB/inch) ≈ 2.3 × f_GHz × √Dk × Df. Standard FR-4: Df = 0.020-0.025 (very lossy). Mid-tier (Megtron 4, IS415): Df = 0.010-0.013. Low-loss (Megtron 6, I-Tera MT40): Df = 0.004-0.006. Ultra-low-loss (Megtron 7, I-Speed): Df = 0.002-0.003. Copper roughness: standard copper (HTE): Rz = 3-6 μm. HVLP (Hyper Very Low Profile): Rz = 1-2 μm. Roughness adds 10-30% to the conductor loss at 25+ GHz. (2) Material selection by data rate: 10 Gbps NRZ (short traces < 6 in): standard FR-4 is usually acceptable. 10 Gbps NRZ (long traces > 10 in): mid-tier (Df ≈ 0.010). 25 Gbps NRZ: low-loss (Df ≈ 0.005) with HVLP copper for traces > 4 in. 56 Gbps PAM4: low-loss or ultra-low-loss (Df < 0.004) with HVLP copper. 112 Gbps PAM4: ultra-low-loss (Df < 0.003), HVLP copper, tight impedance control. (3) Loss comparison at 14 GHz (56 Gbps PAM4 Nyquist), 1 inch trace: FR-4 (Df 0.020): approximately 1.2 dB/inch. Megtron 6 (Df 0.004): approximately 0.45 dB/inch. Megtron 7 (Df 0.002): approximately 0.30 dB/inch. Over a 6-inch trace: FR-4 = 7.2 dB vs Megtron 6 = 2.7 dB. The 4.5 dB difference is critical in a channel with a 30 dB total budget. (4) Cost: standard FR-4: ~1× (baseline). Mid-tier (Megtron 4, IS415): 1.5-2.5×. Low-loss (Megtron 6): 2.5-4×. Ultra-low-loss (Megtron 7): 4-8×. The cost premium is per panel, affecting the entire board cost.

Category: Signal Integrity and High Speed Digital

Updated: April 2026

Product Tie-In: PCB Materials, Connectors, Test Equipment

PCB Material for High Speed

PCB material selection is one of the most impactful decisions in high-speed design, directly determining the achievable data rate and trace length for a given channel loss budget.

Material Vendors

(1) Panasonic: Megtron 4 (R-5775N): mid-tier, Df 0.010. Megtron 6 (R-5775K): low-loss, Df 0.004. Megtron 7 (R-5785N): ultra-low-loss, Df 0.002. (2) Isola: IS415: mid-tier, Df 0.012. I-Tera MT40: low-loss, Df 0.005. I-Speed: ultra-low-loss, Df 0.003. (3) Rogers: RO4350B: low-loss, Df 0.004 (RF-grade, used for mixed RF/digital). RO3003: ultra-low-loss, Df 0.001 (premium, primarily for RF applications). (4) Hybrid stackups: many designs use a mix of materials (low-loss for signal layers, FR-4 for power/ground) to reduce cost while maintaining signal integrity on the critical layers.

PCB Material Properties

Loss ≈ 2.3 × f(GHz) × √Dk × Df (dB/inch)
FR-4 (Df 0.020): ~1.2 dB/inch at 14 GHz
Megtron 6 (Df 0.004): ~0.45 dB/inch at 14 GHz
HVLP copper: Rz < 2 μm (vs 3-6 μm standard)
Cost: 2.5-8× premium for low-loss laminate

Common Questions

Frequently Asked Questions

Can I mix materials in the same stackup?

Yes. Hybrid stackups are common and cost-effective. Signal layers (high-speed SerDes): use low-loss laminate (Megtron 6). Power/ground layers: use standard FR-4. Consideration: the different Dk values between layers must be accounted for in the impedance design. The lamination compatibility (CTE, glass transition temperature) must be verified with the PCB fabricator.

How important is copper roughness?

At 5 GHz: roughness contributes approximately 10% of the total conductor loss. At 25 GHz: roughness contributes 20-40% of the total conductor loss. Using HVLP copper (Rz < 2 μm) instead of standard HTE (Rz 5 μm): saves approximately 10-20% of the total trace loss at 25 GHz. For 56+ Gbps designs: HVLP copper is mandatory (the roughness loss is too significant to ignore).

How do I verify the PCB material performance after fabrication?

Request test coupons on the production panel. Measure insertion loss vs frequency using a VNA with appropriate fixtures (PCB launches). Compare the measured loss to the simulation (which uses the specified Dk and Df). The measured loss should agree within ±10% of the simulation. If significant discrepancy: investigate the material Dk/Df (request material test reports from the fabricator), the copper roughness (SEM cross-section), and the impedance (TDR measurement on the coupon).

Keep Reading