Projects & circuits

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.

Advertisement

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

Each value comes from the cited formula, worked through on our full layout guide. Copper is 1 oz (35 µm), the rise is 10 °C, and FR-4 is taken as εr 4.5.
RuleNumberBasis
Signal trace (our default)0.25 mmFine for logic and slow signals
Trace and space, fab minimum0.10 mm (2-layer), 0.09 mm (multilayer)JLCPCB, 1 oz copper
Trace and space we design to0.15 mmMargin for any low-cost fab
Power trace, outer layer0.30 mm for 1 A, 0.78 mm for 2 A, 1.37 mm for 3 A, 2.77 mm for 5 AIPC-2221, 10 °C rise
Power trace, inner layer0.78 mm for 1 A, 2.03 mm for 2 AAbout 2.6 times the outer width
Via0.3 mm hole, 0.6 mm pad, about 1.35 A eachFab minimum 0.15 mm / 0.25 mm
50 Ω microstrip2.88 mm on 2 layers, 0.38 mm on 4 layers1.53 mm and 0.2 mm to the plane, εr 4.5
100 nF decoupling capacitorWithin 2 mm of the power pin2.3 nH, 1.4 Ω at 100 MHz
Silkscreen0.15 mm line, 1.0 mm text heightJLCPCB minimum
outerinner0.5 A0.12 mm0.30 mm1 A0.30 mm0.78 mm2 A0.78 mm2.03 mm3 A1.37 mm3.56 mm5 A2.77 mm7.19 mm
Figure 1. Trace width against current on 1 oz copper at a 10 °C rise. Inner layers lose heat more slowly, so they need about 2.6 times the width.
JLCPCBourstrace and space0.10 mm (0.09 mm multilayer)0.15 mmvia hole0.15 mm0.30 mmvia pad0.25 mm0.60 mm
Figure 2. JLCPCB's minimums beside the values we design to, drawn to scale. The extra margin lets any low-cost fab make the board.

Pages in this section

Advertisement

Lessons behind these pages

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.

Should I use a two-layer or four-layer PCB? Two layers suit slow, simple boards. Pick four when the board has a USB or Ethernet port, RF, a fast clock or a dense microcontroller layout, because the inner ground plane gives every signal a short return path.

How close should a decoupling capacitor be to the IC? Within about 2 mm of the power pin. At 2 mm the loop is about 2.3 nH and 1.4 Ω at 100 MHz; at 10 mm it is 10.5 nH and 6.6 Ω, nearly five times worse.

Sources: IPC-2221B (trace and via current), Hammerstad and Jensen 1980 (microstrip), JLCPCB PCB capabilities (checked 31 Oct 2026).

Advertisement