On this page · 10 sections
- 01What is a PCB stack-up?
- 02What rules make a good stack-up?
- 03What is the best 4-layer stack-up?
- 04Which 6-layer stack-up should you use?
- 05When do you need 8, 10 or 12 layers?
- 06How does copper weight change the stack-up?
- 07Which material and Tg should a multilayer board use?
- 08How do you specify controlled impedance?
- 09What should you tell your fabricator about the stack-up?
- 10Why confirm the stack-up before routing?
Building this board?
A multilayer stack-up fixes your impedance, your EMC behaviour and a good part of your cost before a single track is routed. Change it after routing and you route again. The good news is that a handful of proven arrangements cover most designs. This guide explains how a stack-up is built, the rules every good one follows, and the 4-, 6- and 8-layer arrangements we see succeed again and again.
What is a PCB stack-up?
A stack-up is the vertical recipe of a multilayer board: which copper layer carries what, and what separates the layers. A multilayer board is built from cores — fully cured laminate with copper on both sides — and prepreg, glass cloth impregnated with partly cured resin. In lamination, heat and pressure melt the prepreg, which flows into the gaps between copper features and cures, bonding the stack into one solid board.
Table 1 · The building blocks
| Element | What it is | Typical values |
|---|---|---|
| Copper | Inner layers are core copper; outer layers start as foil and are plated up | 1 oz = 35 µm; outer layers often 0.5 oz foil plated to about 1 oz |
| Core | Cured FR-4 laminate with copper on both sides | From about 0.1 mm to 1.2 mm |
| Prepreg | Glass cloth plus uncured resin that bonds the stack | Styles 106, 1080, 2116, 7628 — about 0.05 to 0.2 mm per ply |
| Dielectric constant (Er) | Sets impedance together with height and width | FR-4 about 4.2–4.6; 4.4 is a common design value |
| Finished thickness | Total after lamination and plating | 0.4 mm to 3.2 mm standard; 0.2 mm for thin rigid designs |
4 LAYERSS/G/P/S
The default: thin prepreg under each signal layer, thick central core.
6 LAYERSS/G/S/P/G/S
The EMC choice: every signal layer has a plane beside it.
8 LAYERSS/G/S/G/P/S/G/S
Fast pairs on L3 and L6, each shielded between two planes.
G groundP powerS signalCopper thickness exaggerated for clarity
What rules make a good stack-up?
Four rules carry almost every design. Break one only when you know exactly what you are trading for it.
- Every signal layer next to a reference plane. Return current flows in the plane directly beneath the track. A signal far from its plane forms a large current loop, which radiates and picks up noise.
- Symmetry about the centre. Mirror copper weights, dielectric thicknesses and copper density from top to bottom. An asymmetric stack bows in lamination and again in reflow.
- Power and ground close together. A thin dielectric between adjacent power and ground planes adds distributed decoupling capacitance and lowers plane impedance at high frequency.
- An even layer count. Boards are built from double-sided cores, so 4, 6 and 8 layers are natural. An odd count costs nearly the same as the next even one and is more prone to warp.
What is the best 4-layer stack-up?
For most designs: Signal / Ground / Power / Signal. Both outer signal layers sit next to a solid plane, the ground plane shields top-side components from the power plane, and the build is symmetric. Keep the outer prepreg thin and put the bulk of the thickness in the central core.
Table 2 · Example 1.6 mm four-layer build
| Layer | Use | Material | Thickness |
|---|---|---|---|
| L1 | Signal and components | Foil plated to about 1 oz | 35 µm |
| — | Prepreg | 7628 | ≈ 0.2 mm |
| L2 | Ground plane | 1 oz copper | 35 µm |
| — | Core | FR-4 | ≈ 1.07 mm |
| L3 | Power plane | 1 oz copper | 35 µm |
| — | Prepreg | 7628 | ≈ 0.2 mm |
| L4 | Signal and components | Foil plated to about 1 oz | 35 µm |
Illustrative. CAM confirms the actual build against the materials in stock before production. Scroll the table sideways →
The thin prepreg between L1 and L2 is what makes this stack work. The closer a track sits to its plane, the narrower it can be for a given impedance and the tighter its field — so less crosstalk and less radiation. The table shows how strongly dielectric height drives a 50 Ω track width.
Table 3 · Approximate 50 Ω outer-layer track width
| Signal-to-plane dielectric | Approx. 50 Ω width |
|---|---|
| 0.10 mm | ≈ 0.14 mm (5.5 mil) |
| 0.20 mm | ≈ 0.33 mm (13 mil) |
| 0.36 mm | ≈ 0.63 mm (25 mil) |
Microstrip, 1 oz copper, Er 4.4, no solder mask, IPC-2141 approximation. Mask lowers impedance by a few ohms; the fabricator's field solver sets the final width.
An alternative four-layer arrangement puts ground on both outer layers and routes signals inside (G / S / S / G). It shields very well but leaves little room for parts and makes rework and probing harder. Most designs are better served by the classic order.
Which 6-layer stack-up should you use?
The common six-layer arrangement, Signal / Ground / Signal / Signal / Power / Signal, gives four routing layers — but its two inner signal layers sit side by side and need orthogonal routing to limit crosstalk. The stronger EMC choice trades one routing layer for a second ground: Signal / Ground / Signal / Power / Ground / Signal. Every signal layer now has an adjacent plane and the power plane is enclosed between grounds. Choose it when the board carries USB, Ethernet, LVDS or a fast memory bus, or has an EMC test to pass.
Table 4 · Two six-layer arrangements
| Arrangement | Routing layers | Strength | Weakness |
|---|---|---|---|
| S / G / S / S / P / S | 4 | Maximum routing | Adjacent inner signal layers; L6 references the power plane |
| S / G / S / P / G / S | 3 | Every signal layer referenced; best EMC | One routing layer fewer |
Scroll the table sideways →
When do you need 8, 10 or 12 layers?
Eight layers is rarely about routing space alone. It is about giving fast signals quiet, plane-shielded inner layers: Signal / Ground / Signal / Ground / Power / Signal / Ground / Signal. Route the fastest pairs on L3 and L6, each between two planes as a stripline, where they neither radiate nor pick up noise. Ten and twelve layers extend the pattern with more plane pairs. We build 4, 6, 8, 10 and 12 layers; beyond eight, agree drill aspect ratio, copper weights and lamination with us early, because thickness rises with every pair.
How does copper weight change the stack-up?
Heavier copper carries more current but costs room in the stack. A 2 oz inner layer is 70 µm thick, and the prepreg beside it must flow into the gaps between its features, so the pressed dielectric ends up thinner than the prepreg's nominal value; the fabricator accounts for this in the stack calculation. Heavy copper also needs wider track and space — roughly 8 / 8 mil at 2 oz — and must be balanced: a 2 oz plane on L2 wants 2 oz on L3. We build 1 oz (35 µm) and 2 oz (70 µm) as standard; 3 oz (105 µm) and heavier on request. If only one rail carries high current, a wide track or a dedicated plane on 1 oz copper is often better than moving the whole stack to 2 oz.
Which material and Tg should a multilayer board use?
Multilayer boards take more heat than two-layer boards: lamination first, then several lead-free reflow passes for double-sided assembly. Tg, the glass transition temperature, marks where FR-4 softens and its Z-axis expansion accelerates. Standard FR-4 has a Tg of about 130–140 °C; mid-Tg grades sit near 150 °C and high-Tg grades near 170–180 °C. For six layers and more, thick boards and lead-free assembly, a Tg 170 °C material keeps plated holes reliable through reflow. Decomposition temperature (Td) matters too: lead-free-capable laminates are rated at 340 °C or more. Our FR-4 comes in Tg 150 °C and Tg 170 °C grades.
How do you specify controlled impedance?
Specify targets, not geometry. Tell your fabricator the impedance, the layer, its reference planes and the tolerance — for example '50 Ω single-ended on L1 referenced to L2; 100 Ω differential on L3; ±10%'. The fabricator solves width and spacing against its real materials and returns the geometry to route with.
- Common targets: 50 Ω single-ended; 90 Ω differential for USB; 100 Ω differential for Ethernet and LVDS.
- What we offer: controlled impedance, ±10% tolerance, with stack-up design support.
- Impedance is normally verified by TDR on test coupons built into the production panel, which share the board's stack-up and process.
- Copy track widths from an application note only if you also copy its exact material, prepreg and copper. Otherwise the number is simply wrong.
What should you tell your fabricator about the stack-up?
- Layer count and the function of each layer: signal, ground, power or mixed.
- Finished board thickness and its tolerance.
- Copper weight per layer — outer and inner layers may differ.
- Material and Tg: FR-4 Tg 150 °C suits most designs; Tg 170 °C suits lead-free assembly with several reflow passes, thick boards and hot service.
- Impedance targets with their layers, reference planes and tolerance.
- Any via structure other than plain through-holes — and ask before you design it in.
Why confirm the stack-up before routing?
Because the stack-up decides your track widths. Route 50 Ω lines at 0.33 mm assuming 0.2 mm prepreg, discover the build uses a thinner one, and every controlled track is wrong. A stack-up confirmed up front costs nothing; one changed after routing costs a re-layout. Send us the layer count, thickness, copper and impedance targets and we return a proposed build with track geometries. Multilayer lead times are quoted per job after engineering review — see multilayer PCB for the full capability.
Written by
S.B. Electronics Engineering Team
The CAM, production and quality engineers at our factory in the Gandhinagar G.I.D.C. Electronics Estate — the people who review incoming data and build the boards. Published ; last reviewed and updated .
