PCB design
Layout rules for two- and four-layer boards. Each rule comes with its formula, so you can check a trace width or a via yourself.
These are the numbers to check before you order a board. On 1 oz outer copper with a 10 °C rise, IPC-2221 gives 0.30 mm for 1 A, 0.78 mm for 2 A and 1.37 mm for 3 A; inner layers need about 2.6 times as much. A 0.3 mm via carries about 1.35 A, so use three for 3 A. A 50 Ω trace is 2.88 mm wide on a 1.6 mm two-layer board and 0.38 mm on a four-layer board with 0.2 mm to the plane. Keep each 100 nF decoupling capacitor within 2 mm of its power pin. JLCPCB will make 0.10 mm trace and space on two layers; we design to 0.15 mm.
The numbers at a glance
| Rule | Number | Basis |
|---|---|---|
| Signal trace (our default) | 0.25 mm | Fine for logic and slow signals |
| Trace and space, fab minimum | 0.10 mm (2-layer), 0.09 mm (multilayer) | JLCPCB, 1 oz copper |
| Trace and space we design to | 0.15 mm | Margin for any low-cost fab |
| Power trace, outer layer | 0.30 mm for 1 A, 0.78 mm for 2 A, 1.37 mm for 3 A, 2.77 mm for 5 A | IPC-2221, 10 °C rise |
| Power trace, inner layer | 0.78 mm for 1 A, 2.03 mm for 2 A | About 2.6 times the outer width |
| Via | 0.3 mm hole, 0.6 mm pad, about 1.35 A each | Fab minimum 0.15 mm / 0.25 mm |
| 50 Ω microstrip | 2.88 mm on 2 layers, 0.38 mm on 4 layers | 1.53 mm and 0.2 mm to the plane, εr 4.5 |
| 100 nF decoupling capacitor | Within 2 mm of the power pin | 2.3 nH, 1.4 Ω at 100 MHz |
| Silkscreen | 0.15 mm line, 1.0 mm text height | JLCPCB minimum |
Pages in this section
- PCB designHow to design a great PCB: the layout rules, with the numbersPCB layout rules with numbers: IPC-2221 trace width, vias, 50 Ω microstrip on 2 vs 4 layers, decoupling distance and fab limits, each from a cited formula.
- PCB manufacturingHow PCBs are made: from your Gerber files to a tested boardHow a PCB is made, step by step: drilling, hole plating, imaging, etching, mask, finish and test, with the copper, plating and tolerance numbers worked out.
Lessons behind these pages
- IC power decouplingWhere the 100 nF goes and why its distance matters.
- Decoupling capacitorsChoosing the value and the dielectric.
- IC packagesDIP, SOIC, QFN: footprints and pitch.
- Regulator thermal designCopper area as a heatsink.
- HeatsinksWhen board copper is not enough.
- Soldering basicsAssembling the board once it arrives.
Calculators and guides
Tips before you route
- Load your fab's rules into the design-rule check before you place the first part. A limit you forgot to set turns into a long list of errors after routing.
- A 0.25 mm trace on a two-layer board is about 135 Ω, not 50 Ω. For short, slow signals it rarely matters. For USB, Ethernet or RF, use four layers and the 0.38 mm width.
- JLCPCB charges extra for 0.1 and 0.15 mm via holes, and for 0.2 or 0.25 mm holes with a pad under 0.45 mm. A 0.3 mm hole with a 0.6 mm pad avoids that and still carries about 1.35 A.
- Push 2 A through 50 mm of 0.25 mm trace and it drops 197 mV and wastes 394 mW. The 0.78 mm width from the table drops 66 mV.
- Run each signal over unbroken ground. On a two-layer board, pour ground on the bottom and keep long traces off it, because a slot in the pour forces the return current to go around.
What we'd do
Our take: For a first board with a microcontroller, a USB port or anything faster than about 20 MHz, pay for four layers. The ground plane sits 0.2 mm under every signal and the 50 Ω width drops to 0.38 mm. For a simple two-layer board, design to 0.15 mm trace and space, 0.3/0.6 mm vias and the outer-layer widths in the table, so any of the low-cost fabs can make it. Then read the full layout guide before you order.
Questions people ask
How wide should a PCB trace be for 1 A? 0.30 mm on an outer layer of 1 oz copper, for a 10 °C rise (IPC-2221). An inner layer needs 0.78 mm for the same current. Add margin if the board sits in a warm box.
What is the minimum trace width a PCB fab can make? JLCPCB lists 0.10 mm trace and space for one- and two-layer boards and 0.09 mm for multilayer, both with 1 oz copper; 2 oz copper needs 0.16 mm. We design to 0.15 mm for margin.
How much current can a via carry? About 1.35 A for a 0.3 mm hole with 18 µm of plating at a 10 °C rise, using the IPC-2221 relation on the barrel's copper. For a power rail, use several vias in parallel: three for 3 A.
Sources: IPC-2221B (trace and via current), Hammerstad and Jensen 1980 (microstrip), JLCPCB PCB capabilities (checked 31 Oct 2026).
