Every PCB design journey eventually hits the point where two layers aren't enough. You need proper ground planes, controlled impedance, and EMI that won't make compliance testing a nightmare. That's where 4-layer boards come in — and choosing the right stackup configuration is the single most consequential decision you'll make.
After manufacturing thousands of 4-layer PCBs, here's what I've learned about getting the stackup right the first time.
The Three Standard Configurations
About 95% of all 4-layer PCBs we manufacture fall into three configurations:
1. Signal-Ground-Power-Signal (S-G-P-S)
The workhorse. Both outer layers carry signals, L2 is a solid ground plane, L3 is your power plane.
Why it works: Top-layer signals sit directly above the ground plane (0.12-0.20mm spacing), creating well-defined microstrip transmission lines. This handles USB 2.0, SPI, I2C, moderate Ethernet, and most microcontroller designs without breaking a sweat.
Production stat: This accounts for roughly 60% of our 4-layer orders.
2. Signal-Ground-Ground-Signal (S-G-G-S)
When signal integrity and EMI take priority over convenient power distribution. Both inner layers serve as ground planes.
Why choose this: Every signal trace on both outer layers references a solid, continuous ground plane. No power plane splits to disrupt return currents. Lower radiated emissions, better signal integrity margins.
Best for: USB 3.0+, HDMI, differential pairs above 1 GHz, designs needing FCC Class B with minimal margin.
3. Ground-Signal-Signal-Ground (G-S-S-G)
Signals on inner layers, ground planes on both outer surfaces. Maximum shielding — a Faraday cage for your traces.
Trade-off: Nearly every component pad needs a via, dramatically increasing via count. Reserved for RF front-ends, precision analog, and military/aerospace applications.
The Material Details Everyone Skips
Here's something most stackup guides miss entirely: the actual materials that constitute your dielectric layers.
Prepreg Types (What Your Fab Actually Uses)
| Style | Cured Thickness | Resin Content | Best For |
|---|---|---|---|
| 106 | 0.05mm/ply | ~70% | Ultra-thin builds (<0.8mm) |
| 1080 | 0.075mm/ply | ~62% | 1.0mm total thickness boards |
| 2116 | 0.12mm/ply | ~52% | Standard 1.6mm boards (most common) |
| 7628 | 0.18mm/ply | ~58% | Maximum Z-axis stability |
For a standard 1.6mm 4-layer board, we typically use a 1.0mm FR-4 core (Shengyi S1141 or ITEQ IT-140) with single-ply 2116 prepreg on each side.
Impedance Control — Real Numbers
Everyone says "impedance control is important" but nobody shows the math. Here's what actually achieves 50Ω on a standard 1.6mm stackup:
- Dielectric: Single ply 2116 prepreg (0.12mm, Dk ~4.25 at 1 GHz)
- 50Ω single-ended trace width: ~0.27mm (10.6 mil)
- 100Ω differential: 0.15mm traces with 0.18mm edge spacing
How prepreg choice changes your trace width target:
| Prepreg | Dielectric | Trace Width for 50Ω |
|---|---|---|
| 1080 (1 ply) | 0.075mm | 0.165mm (6.5 mil) |
| 2116 (1 ply) | 0.12mm | 0.27mm (10.6 mil) |
| 7628 (1 ply) | 0.18mm | 0.35mm (13.8 mil) |
The 2116 single-ply option sits in the sweet spot — trace widths neither too narrow for reliable etching nor too wide for reasonable routing density.
Standard vs Custom Stackups: The Cost Reality
This is where most engineers lose money unnecessarily.
Standard stackup: Uses materials already in stock, established press recipes, verified impedance data. Boards enter production immediately.
Custom stackup triggers: Unusual thickness (0.6mm, 1.4mm), specific prepreg not in standard builds, non-standard copper weights, mixed materials.
Cost impact of custom: +15-25% unit cost on prototypes, +2-5 business days lead time. For production (100+ pcs), the premium drops to 5-10%.
Pro tip: Before finalizing your design, request your manufacturer's standard stackup library. If your impedance targets work with standard dielectric thicknesses, you capture full cost and time savings.
Stackup Specification Template
Stop sending "4 layers, 1.6mm, FR-4" to your fab. Here's what they actually need:
STACKUP SPECIFICATION
Total thickness: 1.60mm ±10%
Layer count: 4
Material: FR-4 Tg >= 150°C
Layer Stack:
L1 - Signal (Top) | 1 oz Cu
Prepreg: 2116 x1 | ~0.12mm | Dk 4.2-4.4
L2 - Ground (GND) | 1 oz Cu | Plane
Core: FR-4 | 1.0mm | Dk 4.2-4.5
L3 - Power (VCC) | 1 oz Cu | Plane
Prepreg: 2116 x1 | ~0.12mm | Dk 4.2-4.4
L4 - Signal (Bottom) | 1 oz Cu
IMPEDANCE:
- 50Ω ±10% single-ended (L1, L4)
- 100Ω ±10% differential (L1, L4)
Common Mistakes We Catch in DFM Review
Asymmetric copper distribution: When one inner layer has 85% copper fill and the other has 30%, differential thermal contraction bows the board. IPC-6012 limit is 0.75% for SMT. Fix: copper balance within 20 percentage points between L2/L3.
Signals crossing ground splits: Return current has no path, creates antenna loops, fails EMC testing. If you must split planes, ensure no signals cross the boundary.
Insufficient antipad clearance: 0.10mm clearance on inner planes leaves zero margin for drill + imaging registration tolerances. Use 0.20mm minimum.
Decision Framework
- Need identical performance on both outer layers? → S-G-G-S
- Need dedicated power plane for multiple voltage rails? → S-G-P-S
- Need maximum shielding from external interference? → G-S-S-G
- Not sure? → S-G-P-S (the safe default for 60% of applications)
This guide is based on production experience manufacturing 4-layer PCBs across thousands of designs. For a deeper dive with full impedance calculations and material specifications, see the complete 4-layer PCB stackup design guide.
Need help with your stackup? AtlasPCB offers free DFM review with impedance modeling for every production order.
