2-layer
- Top: signals / components; bottom: signals / GND pour.
- Only option for very cheap boards — poor EMI, poor SI above 50 MHz.
- Make bottom layer a continuous ground pour wherever possible.
4-layer (common)
| Layer | Use |
|---|---|
| Top | Signal + components |
| L2 | Solid GND plane |
| L3 | Power plane (or second GND + routed power) |
| Bottom | Signal + components |
6-layer
| Layer | Use |
|---|---|
| Top | Signal |
| L2 | GND |
| L3 | Signal (routed between planes for SI) |
| L4 | Power |
| L5 | GND |
| Bottom | Signal |
8-layer (typical BGA-heavy)
| Layer | Use |
|---|---|
| Top | Signal + BGA escape |
| L2 | GND |
| L3 | Signal |
| L4 | Power |
| L5 | Power |
| L6 | Signal |
| L7 | GND |
| Bottom | Signal |
Rules of thumb
- Reference plane under every signal layer: ideally GND, or power with plenty of decoupling.
- Symmetric stackup: balance copper on both sides to prevent warpage.
- Signal-signal adjacent layers: route orthogonally to minimize crosstalk.
- Controlled impedance: trace width/height determined by the specific stackup — ask fab for their dielectric thickness.
Worked example: why four layers help
Characteristic impedance of a microstrip depends mainly on the ratio of trace width to the distance to its reference plane. Using the IPC-2141 approximation Z = 87 / √(εr + 1.41) × ln(5.98h / (0.8w + t)) for FR-4 with εr about 4.4 and 1 oz copper (t = 0.035 mm):
- On a 2-layer 1.6 mm board with the ground on the opposite face, h is about 1.5 mm and a 50 ohm trace comes out near 2.8 mm wide, which is impractical for routing.
- On a 4-layer board with a ground plane 0.2 mm below the top layer, the same 50 ohm trace is roughly 0.3 to 0.4 mm wide, a normal routing width. Field solvers differ from this approximation by several percent, so use your fabricator stackup data for the final numbers.
The tight spacing to the plane also cuts loop area and crosstalk, because the return current flows directly under the trace.
Choosing a stackup
- Start with the signals, not the layer count. Count the fast interfaces (DDR, USB, Ethernet, high-speed serial) and the BGA pitch. Fine-pitch BGAs usually force six or more layers just for escape routing.
- Keep plane pairs close. A power plane next to a ground plane separated by a thin dielectric adds small but useful high-frequency decoupling capacitance.
- Avoid splitting the reference plane under fast signals. A trace that crosses a gap in its return plane forces the return current to detour, which creates EMI and ringing.
- Ask the fabricator early. They have standard stackups with known dielectric thicknesses and can quote impedance control. Using their stackup avoids a respin.
- Total thickness is a constraint. Standard boards are 1.6 mm. More layers mean thinner dielectrics between them, not thicker boards, unless you specify otherwise.
Was this article helpful?