Prepreg — the partially cured fiberglass-reinforced epoxy sheet that bonds copper layers together during PCB lamination — is arguably the most consequential material choice in a multilayer PCB stackup. Yet most design documentation leaves it entirely to the fabricator's discretion.
This matters because prepreg simultaneously determines three critical parameters: the finished dielectric thickness between copper layers (which directly sets impedance), the effective dielectric constant at your operating frequency (which sets signal velocity), and the mechanical properties that govern registration accuracy and thermal reliability.
The Problem: "Same Thickness" ≠ Same Performance
A fabricator choosing between one sheet of 7628 prepreg and two sheets of 1080 prepreg to achieve the same nominal thickness will produce boards with measurably different impedance values, different signal propagation delays, and different susceptibility to glass-weave-induced timing skew — all while technically meeting your dimensional tolerance spec.
If you've ever received production boards with impedance 3-5 ohms off from your prototype run (which used a different fab shop), prepreg substitution is likely the culprit.
Glass Weave Styles: Quick Reference
| Style | Pressed Thickness | Typical RC% | Best For |
|---|---|---|---|
| 106 | 0.038-0.050mm | 70-75% | HDI buildup layers, ultra-thin dielectrics |
| 1080 | 0.060-0.070mm | 62-68% | High-speed digital (workhorse for 10-28 Gbps) |
| 2116 | 0.100-0.120mm | 50-56% | Standard multilayer (cost-efficient, adequate for <3 GHz) |
| 7628 | 0.175-0.200mm | 42-48% | Thick dielectric buildup, power planes |
The numbers come from real production data — your actual pressed thickness varies with lamination pressure, resin flow into adjacent copper patterns, and the specific resin chemistry.
Why Resin Content Changes Your Impedance
The two constituent materials in prepreg have dramatically different dielectric constants:
- E-glass fiber: Dk ≈ 6.2-6.6 at 1 GHz
- Epoxy resin: Dk ≈ 3.2-3.5 at 1 GHz
A 1080 prepreg with 65% resin content produces composite Dk ≈ 3.9, while the same glass style with 55% resin content yields Dk ≈ 4.2. That 0.3-unit Dk difference translates to approximately 2-3 ohms shift in 50-ohm impedance.
The practical implication: specifying a generic "dielectric thickness" without constraining resin content creates a situation where the fabricator's material selection shifts your impedance in ways that aren't visible until TDR measurement.
The Glass Weave Effect: Your Hidden SI Problem
Standard glass weaves create a periodic pattern where fiber bundles cross over each other, leaving resin-rich windows between them. A trace running over a glass knuckle sees higher Dk; a trace over a resin window sees lower Dk. This creates position-dependent impedance variation of 2-5 ohms depending on the glass style.
For differential pairs, this is catastrophic at high data rates. If one trace sits over glass and its complement sits over resin, the velocity difference creates intra-pair skew. At 28 Gbps NRZ (35.7ps UI), a 100mm trace with 0.5-unit Dk difference produces 8-12ps skew — that's 25-35% of your bit period gone before you even consider your channel's insertion loss.
Three Mitigation Strategies
1. Diagonal routing (free, wastes routing area)
Route traces 5-15° off the warp/fill axes to average out Dk variation.
2. Spread-glass prepreg (15-25% material premium, eliminates the problem)
Mechanically flattened weave reduces Dk variation to <0.1 units across the weave period.
3. Non-woven / RCC (highest cost, exotic)
For 56+ Gbps applications where even spread-glass isn't sufficient.
How to Specify Prepreg Without Over-Constraining
The right level of specification depends on your performance requirements:
Below 5 GHz (±10% impedance): Specify thickness and material family. Let the fab choose.
5-15 GHz (±7% impedance): Specify glass style and ply count for impedance-critical layers: "Layer 2-3 dielectric: 1x1080 prepreg, 65%±3% RC, pressed thickness target 0.065mm."
Above 15 GHz (±5% impedance): Specify spread-glass, exact laminate system, target Dk at frequency, and require formal stackup review before tooling.
Cost Optimization Tips
From our fabrication experience running thousands of impedance-controlled stackups:
- Use spread-glass only where it matters (signal-to-reference dielectric layers), not everywhere
- Two sheets of 1080 cost 30-40% more than one sheet of 2116 for similar thickness — but the impedance uniformity improvement is often worth it above 5 GHz
- Design around your fab's standard inventory (they stock 4-6 prepreg configs) to avoid MOQ premiums and lead time extensions
- Always provide copper coverage data per layer — it helps the fab calculate resin flow accurately and reduces impedance surprises
The Takeaway
Prepreg selection is where material science meets signal integrity meets manufacturing economics. For designs above a few GHz, leaving it unspecified is leaving your impedance to chance.
The fix is straightforward: include prepreg construction in your fab notes for critical layers, provide copper coverage data, and have a stackup conversation with your fabricator before production — not after you get boards back with impedance outside your budget.
This article is based on fabrication data from impedance-controlled multilayer production. Originally published at AtlasPCB Engineering Blog.
Need help selecting the right prepreg construction for your high-speed design? Our process engineering team reviews stackups and recommends material configurations as part of our PCB manufacturing service.
Top comments (0)