How many layers does your PCB need? A guide to layers and materials

The layer count, the board thickness and the material are three decisions you make very early in PCB design, but their consequences stay with you until series production. They affect the price, electromagnetic compatibility (EMC), signal integrity and how much time you spend on the layout. In this guide we explain how to decide without guesswork.

Single-layer, two-layer, four-layer or more

Most boards we see in practice fall into one of four groups:

A rule of thumb: if the board has a microcontroller clocked above a few tens of MHz, a wireless module, USB or a switching regulator, four layers almost always pay off. For small series the price difference is a few euros per board, while the savings in EMC testing and extra iterations are far greater.

A two-layer board remains an excellent choice for simple analogue circuits, power adapters, breakout boards and anything with enough space and low frequencies.

The standard four-layer stackup

With four layers the most common arrangement is:

1. Top layer: components and signals
2. Layer 2: continuous ground (GND)
3. Layer 3: power (or a second ground)
4. Bottom layer: signals and components

The key to good performance is a ground plane directly below the top signal layer. Every signal then has a short return path, which reduces radiation and crosstalk. On more demanding boards the signal / GND / GND / signal arrangement is gaining ground: power is routed as wide traces on the outer layers, which gives the best EMC behaviour.

With six layers you gain two additional inner signal layers surrounded by ground planes – ideal for sensitive or high-speed signals.

Board thickness

The standard thickness is 1.6 mm, and it is the cheapest because every manufacturer keeps it in stock. Other common thicknesses are 0.4, 0.6, 0.8, 1.0, 1.2, 2.0 and 2.4 mm.

When to choose a different thickness:

• 0.8 to 1.0 mm for small modules, wearables and wherever weight or height matters.
• 0.6 mm or less for modules soldered onto another board (castellated edges) and for more flexible applications.
• 2.0 mm or more for mechanically stressed boards, large connectors, high-current power boards and boards that act as a structural element.

Thickness also affects the aspect ratio of vias (depth to diameter). On a 1.6 mm board a 0.3 mm hole is no problem; on a 2.4 mm board it is already close to the limit that many manufacturers set at a ratio of 8:1 or 10:1.

Copper weight

The thickness of the copper foil is given in ounces per square foot (oz) or in micrometres:

Thicker copper means higher current capacity and better heat dissipation, but also larger minimum clearances and widths (thicker copper cannot be etched as precisely). With 2 oz copper, plan for at least 0.2 mm width and clearance. To estimate the required trace width use a calculator based on IPC-2221 or IPC-2152; as a rough guide, for 1 oz copper and a 10 °C temperature rise, about 1 mm of width per 1 A on an outer layer.

Materials: FR-4 and the glass transition temperature (Tg)

FR-4 is a glass-fibre reinforced epoxy laminate and covers more than 90 per cent of all boards. The key value when choosing it is Tg (glass transition temperature) – the temperature at which the material changes from a rigid to a softer, rubbery state:

• Standard Tg of 130 to 140 °C: sufficient for most consumer and industrial electronics.
• Medium Tg of 150 °C: a common choice for lead-free soldering and for boards that run warmer.
• High Tg of 170 to 180 °C: for automotive and power electronics, multilayer boards with several reflow cycles and applications with high operating temperatures.

In a lead-free reflow process the board reaches 245 to 260 °C. A material with a higher Tg expands less in the Z direction, which reduces the risk of damaged vias. For boards with four or more layers, a Tg of 150 or higher is the recommended choice.

Other materials:

• Aluminium core (MCPCB) for LED lighting and power modules where heat dissipation is critical; almost always single-layer.
• Rogers, Taconic and similar RF laminates for antennas and high-frequency circuits above a few GHz, where a stable dielectric constant matters more than price.
• Polyimide (flex) for flexible and rigid-flex boards.

Surface finish

The surface finish protects the exposed copper and affects soldering:

• HASL (lead-free): the cheapest and robust, but uneven; less suitable for fine-pitch packages (0.4 mm pitch).
• ENIG (electroless nickel immersion gold): flat, long shelf life, suitable for fine pitch and BGA; the standard choice for professional boards.
• OSP: an organic coating, cheap and flat, but with a short shelf life before soldering.
• Immersion silver/tin: an alternative for special requirements.

For small series with SMT assembly we recommend ENIG, as the flat surface works very well for stencil paste printing.

Controlled impedance basics

When you route USB 2.0 (90 Ω differential), Ethernet (100 Ω differential), HDMI, LVDS or RF signals (50 Ω) on a board, the trace impedance must be defined. It is determined by:

• the trace width,
• the distance to the reference plane (ground),
• the dielectric constant of the material (about 4.2 to 4.6 for FR-4),
• the copper thickness and the presence of solder mask.

On a 1.6 mm two-layer board a 50 Ω microstrip would have to be about 2.8 mm wide, which is unusable in practice. On a four-layer board with ground on layer 2 and a prepreg of about 0.1 mm, the same impedance is reached at a width of about 0.17 mm. This is one of the main reasons why high-speed signals need four layers.

When you order controlled impedance, the manufacturer offers its own stackup with exact prepreg and core thicknesses; you then calculate the trace widths with a calculator (e.g. Saturn PCB Toolkit or the built-in tool in Altium or KiCad), or the manufacturer adjusts the widths itself.

How to decide in practice

1. List the fastest signals and interfaces on the board. If any of them has an impedance requirement, choose at least four layers.
2. Estimate the density: fine BGAs and QFNs with many pins are almost impossible to route on two layers.
3. Check the currents: above 5 A consider 2 oz copper or wide copper areas on several layers.
4. Consider the environment: high temperatures and automotive requirements mean a higher Tg.
5. Check the price: for prototypes the difference between two and four layers is often smaller than you might expect.

Need help?

In every electronics development project at Selektronik we propose a stackup that suits the signals, currents and budget – and we manufacture the board too. If your files are ready, choose the layer count, thickness and surface finish in our PCB configurator and see a price estimate immediately. For advice on the layer count or controlled impedance, write to us at info@selektronik.si.