← Journal Hardware · · 6 min

Choosing a 4-layer PCB stackup for connected devices

How to choose a 4-layer PCB stackup for a small connected device: layer order, trace impedance, radio keep-outs and what to tell the fab.

Milo Perović
Founder & lead engineer

  • Architecture
  • DFM
  • EMC
  • RF
Choosing a 4-layer PCB stackup for connected devices

Most connected devices we see end up on four copper layers, yet the 4-layer PCB stackup is often whatever the fab offered as its default, chosen in a dropdown the night the boards were ordered. That works until the radio underperforms or the USB port fails an emissions scan.

This post is for hardware engineers and technical founders laying out a small IoT board: a microcontroller or radio module, a few sensors, a battery charger, maybe USB-C. It covers layer order, dielectric thickness and what to write on the fabrication drawing.

When two layers stop being enough

Two-layer boards are cheap and perfectly good for simple, slow designs. The trouble starts when you route signals on both sides and the ground ends up as a patchwork of pours stitched together with vias. Return currents take long detours and loop areas grow.

We move to four layers when a design has any of the following:

  • A 2.4 GHz or sub-GHz radio with a PCB antenna or a 50 Ω feed to a connector.
  • USB 2.0 data lines, or any other differential pair with an impedance target.
  • A switching regulator sitting close to sensitive analogue inputs or the radio.
  • A fine-pitch part (QFN with a large pad count, or a small BGA) that is hard to escape on two layers.

The price gap between two and four layers at prototype quantities is now small compared with one extra respin.

Layer orders for a 4-layer PCB stackup

There are three common arrangements. The labels below run from top (L1) to bottom (L4).

OrderStrengthsWeaknesses
Signal / GND / Power / SignalThe classic default. L1 has a tight ground reference. Power plane makes distribution easy.L4 references a power plane, so signals changing layers need stitching capacitors or careful planning.
Signal / GND / GND / SignalBoth outer layers reference ground. Layer changes only need a nearby ground via. Very forgiving.Power is routed as wide traces or pours on the outer layers, which costs routing space.
GND / Signal / Signal / GNDGood shielding of inner signals.Hard to probe, rework and debug. Components still need outer-layer pads, which chop up the ground.

For small connected devices we usually choose Signal / GND / GND / Signal, or Signal / GND / Signal-plus-power-pours / Signal with the third layer kept mostly ground. These boards rarely have enough rails to justify a power plane, and a 3.3 V rail plus a battery node fit comfortably as short, wide pours.

Why the return path decides it

At high frequencies, return current flows in the plane directly beneath the trace. When a signal drops through a via from L1 to L4, its return current has to move from L2 to whatever plane L4 references. If both are ground, a ground via next to the signal via gives it a short path. If L3 is a power plane, the return has to cross through the nearest decoupling capacitor, which may be several millimetres away. That detour is a loop antenna, and it shows up in radiated emissions scans.

Dielectric thickness and trace impedance

A typical 1.6 mm 4-layer board has thin prepreg between L1 and L2, a thick core in the middle, and thin prepreg again between L3 and L4. Common prepreg thicknesses sit roughly between 0.1 and 0.2 mm, with the core making up the remainder. The exact figures depend on the fab’s standard build and the glass styles it stocks.

That thin outer dielectric is what sets your microstrip widths. On standard FR-4 with a relative permittivity around 4.2 to 4.6:

  • With about 0.2 mm to the ground layer, a 50 Ω microstrip is roughly 0.3 to 0.37 mm wide.
  • With about 0.1 mm, it drops to roughly half that, which is much easier to bring into a module pad or a U.FL connector.
  • USB 2.0 wants about 90 Ω differential. On a thin prepreg this lands at trace widths and gaps that are easy to route between small components.

Treat these as starting points only. Use the fab’s own impedance calculator with its real dielectric values, and include solder mask in the calculation because it lowers impedance slightly. For RF feeds we often prefer grounded coplanar waveguide: ground pour on both sides of the trace, stitched to L2 with vias, which keeps fields contained.

Board thickness changes everything

Wearables and compact sensors often move to 1.0 or 0.8 mm boards. The layer order stays the same, but the dielectric values change, so every impedance-controlled trace has to be recalculated. A common mistake is copying a layout from a 1.6 mm reference design onto a thinner board and keeping the old trace widths. The feed line then sits well off 50 Ω, and radio range suffers for no visible reason.

Planning the planes around the radio and power

A good stackup can still be undone by what you put on it. A few rules we apply on almost every board:

  1. Keep L2 solid. No traces on the ground layer, and no slots under fast signals. If you must route on L2, do it in a corner where nothing crosses above.
  2. Respect the antenna keep-out on every layer. A chip or PCB antenna needs copper removed beneath it on all four layers, not only the top. Our post on PCB antenna placement for small connected devices covers this in more detail.
  3. Stitch the edges. A row of ground vias along the board outline, and around the RF section, ties the ground layers together and reduces edge radiation.
  4. Keep switching nodes small and on top. The buck converter’s switch node and inductor should sit on L1 directly over solid ground, with the input capacitor loop as tight as possible.
  5. Avoid splitting ground into analogue and digital. On small boards, one continuous ground with sensible component placement nearly always beats split planes.

When to go to six layers

Six layers make sense when you have a BGA processor with external DDR memory, an embedded Linux module with many high-speed interfaces, a cellular modem with several RF paths, or simply too many signals to fit on two outer layers without breaking up the ground. A common six-layer build is Signal / GND / Signal / Power / GND / Signal, which gives every signal layer an adjacent reference.

For a typical ESP32-S3, nRF52840 or STM32L4 based device with a handful of sensors, four layers is nearly always sufficient. If a board like that feels crowded, review placement before adding layers.

What to put on the fabrication drawing

If the fab drawing does not specify the build, the board house will use its default, which may not match what you calculated against. We specify:

  • Finished board thickness and tolerance.
  • Layer order with the function of each layer, matching the Gerber file names.
  • Copper weights, typically 1 oz outer and 0.5 or 1 oz inner.
  • The dielectric build you designed for, or the fab’s named standard stackup.
  • Impedance-controlled nets with target values and tolerance, usually ±10%, and whether you want test coupons.

Controlled impedance adds modest cost, but for a board with a radio feed or USB it is worth paying for.

What we would do on a new board

We settle the stackup with the placement plan, before routing starts:

  • Pick Signal / GND / GND / Signal unless you have a clear reason for a power plane.
  • Get the fab’s actual stackup and permittivity before calculating any widths.
  • Recalculate every controlled trace when the board thickness changes.
  • Place a ground via next to every signal via that changes layers.
  • Clear copper under the antenna on all layers and stitch the RF section.
  • Write the stackup and impedance requirements on the fab drawing, explicitly.

Then check it all again in a structured hardware design review before you order boards. Stackup mistakes are cheap to fix in CAD and expensive to fix once the first batch has arrived.

Working on something similar?Free scoping call →