RF PCB Stackup Planning

4-Layer Megtron 6 Stackup | Low-Loss Digital RF

A practical 4-layer Megtron 6 stackup guide covering dielectric thicknesses, impedance targets, copper roughness impact, and annular ring rules for 25 Gbps+ digital and RF applications.

Cross-section of a 4-layer PCB stackup showing copper layers and dielectric

What Is a 4-Layer Megtron 6 Stackup?

A 4-layer Megtron 6 stackup uses Panasonic’s R-5775N (Megtron 6) ultra-low-loss laminate as the core and prepreg dielectric in a signal–ground–ground–signal or signal–ground–power–signal arrangement. With a published Dk of 3.71 and Df of 0.002 at 12 GHz, Megtron 6 bridges the gap between standard FR-4 and exotic PTFE materials, making it the workhorse choice for 25–56 Gbps NRZ/PAM4 serial links, backplane daughter cards, and moderate-frequency RF front-ends up to Ku-band.

This guide walks through a recommended layer-by-layer build, impedance geometry, copper roughness loss, drill and annular ring constraints, and the trade-offs that determine whether Megtron 6 is the right call for your next board. For a deeper look at the material family itself, see the Panasonic Megtron 6 and 7 fabrication overview.

Recommended 4-Layer Stackup

Differential pair traces on a high-frequency laminate PCB surface

The most common 4-layer Megtron 6 build targets a finished board thickness of 1.6 mm (63 mil) with 50 Ω single-ended and 100 Ω differential impedance on the outer layers. The table below shows a production-proven arrangement.

Layer Function Copper Weight Dielectric Below Thickness (mil / mm)
L1 Signal (microstrip) 1 oz (1.4 mil) R-5680N prepreg 4.0 / 0.10
L2 Ground plane 1 oz R-5775N core 47.0 / 1.19
L3 Power plane 1 oz R-5680N prepreg 4.0 / 0.10
L4 Signal (microstrip) 1 oz — —

Total dielectric stack ≈ 55 mil; with four copper layers and plating, finished thickness lands near 62–63 mil. The thin prepreg on L1–L2 and L3–L4 keeps microstrip trace widths manageable—roughly 4.0 mil (0.10 mm) for 50 Ω single-ended with 1 oz copper after etch, and about 3.8 mil traces on 7.0 mil pitch for 100 Ω differential pairs.

Why Signal–Ground–Power–Signal?

Placing both reference planes adjacent to the thick core gives three advantages: the core’s tight thickness tolerance (±0.5 mil on standard 47 mil core) locks impedance more tightly than prepreg alone; the L2–L3 cavity provides a low-inductance power-ground capacitor; and both signal layers get an unbroken reference plane directly beneath them, minimizing return-path discontinuities.

If your design is purely RF with no power distribution, a signal–ground–ground–signal variant using two thin cores and a single prepreg bond-ply between the grounds can further tighten impedance symmetry between L1 and L4. Consult a free stackup consultation to model either option before committing to fabrication.

Megtron 6 Electrical Properties at a Glance

Parameter Megtron 6 (R-5775N) Standard FR-4 Megtron 7 (R-5785N)
Dk @ 12 GHz 3.71 ~4.2–4.5 3.37
Df @ 12 GHz 0.002 0.018–0.025 0.001
Tg (DSC) 185 °C 130–170 °C 200 °C
CTE-z (50–260 °C) 2.4 % 3.0–3.5 % 1.6 %
Typical use case 25–56 Gbps, RF to Ku-band ≤10 Gbps, general digital 56–112 Gbps, mmWave

Megtron 6’s Df of 0.002 cuts dielectric loss roughly 10× compared to mid-grade FR-4. For designs pushing past 56 Gbps PAM4 or reaching into Ka-band frequencies, stepping up to a Megtron 7 stackup halves the loss again—but at roughly 1.5–2× the laminate cost.

Copper Roughness and Its Impact on Insertion Loss

At 10 GHz and above, conductor loss often dominates over dielectric loss, and copper surface roughness is the biggest variable. Megtron 6 laminates are available with several foil options: standard electrodeposited (ED) copper (Rz ≈ 5–7 µm), reverse-treated foil (RTF, Rz ≈ 2–3 µm), and very-low-profile (VLP) foil (Rz ≈ 1.5 µm). Choosing VLP foil on a 4-layer Megtron 6 stackup can reduce total insertion loss by 0.3–0.5 dB/inch at 14 GHz compared to standard ED foil—a significant margin on a 10-inch backplane trace.

Use the calculator below to estimate the additional conductor loss contributed by your chosen foil roughness. Enter the RMS roughness height, frequency, and trace geometry to see the roughness-induced loss adder in dB/inch.

Loading Copper Roughness Loss Tool…

For example, with VLP foil (Rz ≈ 1.5 µm, RMS ≈ 0.6 µm) at 14 GHz on a 4 mil microstrip, the tool shows roughly 0.08 dB/inch of roughness-added loss. Switch to standard ED foil (RMS ≈ 2.5 µm) and that jumps to about 0.25 dB/inch. Over a 6-inch differential pair, the difference is nearly 1 dB—enough to close or open an eye at 28 Gbps NRZ. Always specify foil grade on your fabrication drawing; if you leave it unspecified, most shops default to standard ED.

Panasonic publishes detailed roughness and loss data in the Megtron 6 product page including Dk/Df versus frequency curves for each foil class.

Annular Ring and Drill Design for Megtron 6

Stacked Megtron laminate sheets showing resin color and copper foil

Megtron 6’s CTE-z of 2.4 % and Tg of 185 °C make it more mechanically stable through reflow than FR-4, but via reliability still depends on proper annular ring sizing. IPC-6012 Class 3 requires a minimum annular ring of 2 mil (0.05 mm) after all registration tolerances. For a standard 10 mil (0.25 mm) drill, that means a minimum pad diameter of 18 mil (0.46 mm) after etch, assuming ±2 mil drill registration and ±1 mil artwork shift.

Check your pad-to-hole geometry against IPC requirements using the annular ring calculator below. Enter your finished hole size, pad diameter, and registration tolerance to confirm compliance.

Loading Annular Ring Checker…

If the tool returns an annular ring below 3 mil for a Class 3 design, increase the pad size or tighten your drill registration specification. On Megtron 6 cores thicker than 40 mil, mechanical drill wander is typically ±1.5 mil at worst; laser-drilled microvias on HDI builds hold ±0.5 mil. For designs requiring microvias in Megtron 6, review the HDI mmWave stackup approach for via-in-pad and stacked microvia rules.

Back-Drill Considerations

In a 4-layer board the through-via stub is short—typically under 50 mil—so back-drilling is rarely needed below 20 GHz. However, if you route high-speed signals on L1 only and the via passes through L4, the ~55 mil stub can resonate near 27 GHz and degrade a 28 Gbps NRZ channel. In that scenario, either use blind vias (L1–L2) or apply a controlled back-drill from the L4 side. Our back-drill depth and stub control guide covers the tolerances and cost impact in detail.

When to Choose Megtron 6 Over Alternatives

Megtron 6 is not always the right answer. Here is a decision framework:

  • Choose Megtron 6 when your channel operates at 10–28 GHz or 25–56 Gbps, you need standard FR-4 processing (no special PTFE bonding or plasma desmear), and your loss budget allows Df ≈ 0.002.
  • Choose Megtron 7 when data rates exceed 56 Gbps PAM4 or frequencies push past 30 GHz; the extra laminate cost buys roughly 3 dB less loss per foot at 28 GHz.
  • Choose PTFE (e.g., Rogers RO4350B) when you need Dk stability within ±0.02 across temperature and frequency for tightly controlled RF impedance, or when your circuit operates above 40 GHz.
  • Choose mid-grade FR-4 when data rates stay under 10 Gbps and cost is the primary driver. Megtron 6 laminate typically costs 3–5× standard FR-4 per panel.

For budget-sensitive RF antenna boards below 6 GHz, a 4-layer Taconic RF-35 stackup delivers acceptable Df at a lower price point than Megtron 6.

Fabrication Notes and Common Pitfalls

Lamination Profile

Megtron 6 prepreg (R-5680N) requires a peak lamination temperature of 200–210 °C with a 60-minute dwell—similar to high-Tg FR-4 but slightly longer. Undercuring causes delamination during lead-free reflow at 260 °C; overcuring raises Dk by up to 0.05. Confirm your fabricator’s press profile matches Panasonic’s published cure schedule.

Impedance Tolerance

Request ±7 % impedance tolerance on controlled-impedance traces. Megtron 6’s Dk variation is ±0.05 (about ±1.4 %), tighter than FR-4’s ±0.15, so the remaining impedance uncertainty comes from etch and dielectric thickness control. A good shop hits ±5 % routinely on 4-layer Megtron 6 boards. Check your target trace widths against the impedance table by material before finalizing artwork.

Solder Mask Over Traces

Liquid photo-imageable (LPI) solder mask adds roughly Dk 3.5–4.0 over microstrip traces, shifting impedance down by 2–4 Ω. Either model the mask in your field solver or specify solder-mask-free zones (mask-defined openings) over critical RF and high-speed differential pairs.

Frequently Asked Questions

Is Megtron 6 suitable for RF applications?

Yes. With Df 0.002 at 12 GHz and stable Dk up to at least 20 GHz, Megtron 6 works well for RF front-end circuits, filters, and antenna feed networks through Ku-band (~18 GHz). Above 30 GHz, PTFE-based laminates or Megtron 7 generally offer better performance.

Can I mix Megtron 6 with FR-4 in the same stackup?

It is possible but not recommended for impedance-controlled layers because the Dk mismatch (3.71 vs. ~4.3) creates different trace widths on adjacent layers and complicates field-solver modeling. If cost forces a hybrid, keep Megtron 6 on the signal-adjacent dielectrics and FR-4 in the non-critical core.

What is the maximum operating frequency for a 4-layer Megtron 6 board?

There is no hard cutoff. Insertion loss becomes the limiting factor: a 4 mil microstrip on Megtron 6 with VLP foil loses roughly 0.7 dB/inch at 20 GHz. If your link budget tolerates that, 20+ GHz is achievable. Beyond 25 GHz, evaluate whether the loss margin still closes or whether Megtron 7 or a PTFE hybrid is needed.

Does Megtron 6 require special drilling or desmear?

Standard mechanical drilling works fine. Desmear uses a permanganate process identical to high-Tg FR-4—no plasma desmear is needed. This is one of Megtron 6’s key advantages over PTFE laminates, which often require sodium-naphthalene etch-back or plasma treatment for reliable plating adhesion.

Ready for a quotation?

Send your requirements for a material, stackup and manufacturing review. Price and schedule are confirmed for your project.

Upload Gerber