Every trace on a circuit board carries current, and a few of them carry enough to matter: the input from the terminal block, the rails of a motor driver, the return from a heater, the string that feeds a metre of LEDs. Those traces are resistors, they make heat, and the board around them is a poor way of getting rid of it. The question of how wide they must be has a standard answer, IPC-2221, that is seventy years old and conservative, a newer one, IPC-2152, that is better and more work, and a set of things around the trace, vias, terminals and the enclosure, that fail before the copper does. This guide is the reasoning behind the trace width calculator.
Copper on a board is a resistor with poor cooling
Copper has a resistivity of 1.72 × 10−8 Ω·m at 20 °C, rising 0.393 % for every degree. A trace 1 mm wide in 1 oz copper, which is 35 µm thick, has a cross-section of 0.035 mm² and a resistance of 0.49 mΩ per millimetre: 50 mm of it is 25 mΩ, 3 A through it drops 74 mV and makes 0.22 W of heat. That is not much power, but it is made in a strip of metal a third of a hair thick, and it has three ways out. It can go upward into the air, by convection and a little radiation, which needs the trace to be on the surface and the air to be free to move. It can conduct sideways and downward into the laminate, which is glass and epoxy with a thermal conductivity of about 0.3–0.4 W/m·K through its thickness, a thousand times worse than copper. Or it can conduct along the copper itself to somewhere cooler: a pad, a pour, a plane.
The trace warms until the heat leaving equals the heat made, and the temperature it settles at above the board is the rise. A rise is chosen, usually 10 °C, and the width follows from it: a wider trace has less resistance, so it makes less heat, and more surface, so it sheds more. Nothing about that is linear, which is why the standards are curves.
The IPC-2221 curve and what k means
The charts in section 6.2 of IPC-2221 relate current, temperature rise and copper cross-section, and a curve fit to them is what every trace width calculator, including ours, computes:
Solved for the area and divided by the copper thickness, 1.378 mil per ounce per square foot, it gives the width. The exponents say something physical: doubling the allowed rise gains only 36 % more current, and doubling the current needs 2.6 times the area, because the resistance falls with area but the surface grows only with the width. The constant k is the cooling. For an external trace it is 0.048, for an internal one half of that, on the reasoning that a trace buried in the laminate has lost the air above it and can only conduct into epoxy. Halving k is the same as doubling the current: an inner trace needs the area an outer trace would need for twice the amps.
The data behind the curves were measured in the 1950s at the US National Bureau of Standards on single traces on bare boards in still air, and were carried through MIL-STD-275 and IPC-D-275 into IPC-2221 essentially unchanged. They know nothing about the thickness of the board, the copper beside and beneath the trace, an enclosure, forced air or altitude. On a modern four-layer board with a ground plane under the trace the real rise is well below the chart; in a sealed box on a wall in June it is above it. The chart is a safe first pass for a trace on a board with little other copper, and a starting point everywhere else.
IPC-2152: the modern picture
IPC-2152, published in 2009, replaced the old curves with measurements on real boards and a method that accounts for what the old data ignored. Its findings are the useful part even if you never open its charts. A copper plane in the board, even one not connected to the trace, spreads the heat and lowers the rise markedly; a thicker board conducts more heat away; internal and external traces on the same board with planes behave much more alike than the factor of two, and the old external curve was in some conditions the optimistic one, not the internal. An enclosure, which takes away the convection, raises the rise; so does altitude, because thinner air cools less, which matters for equipment going to Skardu or Gilgit. Solder mask makes little difference.
Spend the time on IPC-2152, or on a thermal simulation, when the trace is genuinely about current: a power converter, a motor driver, a battery board, anything above a few amps or in a sealed enclosure at a high ambient. For the rest, IPC-2221 with a 10 °C rise leaves enough margin that the board will be limited by something else first, and that something is the next section.
Vias, connectors and terminals: the weakest link is not the trace
A via is a hole with a thin tube of plated copper in it. A 0.3 mm hole with 25 µm of plating, which is what IPC-6012 class 2 requires as a minimum, has a copper cross-section of about 24 000 µm², 37 mil², which the same curve puts at 1.8 A on the surface and 0.9 A inside at a 10 °C rise. As a rule of thumb, and it is only that, count about 1 A per such via and use several in parallel for any connection that carries real current: a row of four or six under a terminal pad, a field of them stitching a pour on the top layer to one on the bottom. Vias in parallel share current well because they are short and their resistance is dominated by the plating, which is the same for all of them.
The terminal is more often the limit than either. A 2.54 mm pin header is rated 1–3 A per contact; a 3.5 mm pluggable terminal block about 8 A; a 5.08 mm screw terminal 10–16 A; a JST-XH crimp contact 3 A; and every one of those ratings assumes the right wire, the right crimp and a clean, tight joint. A 20 A trace into a 10 A terminal is not a design; nor is a wide trace narrowing to a thermal-relief spoke at the pad. Check the mating parts, the wire and the crimp before widening the copper, and if the current is above what a board terminal is rated for, take it off the board: a ring lug on a stud, a bus bar, a cable that bypasses the board altogether.
Voltage drop and sense lines
For a power trace the drop is rarely the issue: 57 mV on a 12 V rail is half a per cent. It matters in three places, and in all three the fix is layout, not width. A current-sense resistor of 10 mΩ that is read by the same traces that carry the current will read the trace as well; 25 mΩ of copper on a 10 mΩ shunt is a 250 % error. The sense lines must leave the shunt from its own pads, inside the current path, in the four-wire or Kelvin pattern, and most shunt footprints have the extra pads for it. An ADC reference or a sensor ground that shares a return path with a load sees the load's current times the return's resistance as an offset that moves with the load; give the measurement its own return to the star point. And an LED string or a heater at the end of a long thin trace is dimmer or cooler than the one at the start: a 5 V, 3 A strip fed through 200 mm of 0.5 mm trace loses 0.3 V, which is visible. The voltage drop calculator does the same arithmetic for the cable that brings the current to the board.
Copper weight, pours and planes
One ounce per square foot, 35 µm, is the default copper on almost every board and the right choice for almost every trace; the calculator's table shows it carrying 3 A at 1.37 mm and 5 A at 2.8 mm at a 10 °C rise, which fits most boards. On a board with plated holes the outer layers gain 20–35 µm of plating on top of the foil, so "1 oz" outer copper is often 50–70 µm finished, and the calculator's use of the nominal foil is on the safe side; the inner layers are the foil alone. Two ounces halves the width for the same current and halves the resistance for the same width, and it is the answer on a small board where 10 A must pass between fine-pitch parts. It costs more, it cannot be etched as finely (the minimum trace and gap roughly double), and its pads need more heat to solder. Half-ounce copper on inner layers is common on fine-pitch boards and needs twice the width for the same current.
Before going to heavier copper, use more of the copper you have. A pour beside a trace helps cool it; a pour on the other side, stitched through with a field of vias, doubles the copper; a power plane on an inner layer is a trace as wide as the board. What fights you is thermal relief: the four thin spokes that connect a pad to a plane so that the plane does not sink the soldering iron's heat. Each spoke is a narrow trace, about 1 A at 0.4 mm on the surface by the same curve, and a pad on a 10 A plane connected through four of them is a 4 A connection. Set the relief rules per net: solid connections or wide spokes for power nets, and accept that those pads need a hotter iron or a preheated board.
The example in numbers
A 3 A supply trace on an outer layer of a 1 oz board for a motor driver: 10 °C rise, 50 mm long, the board at 25 °C, and a 1.0 mm width already drawn because it fits between two connector pins.
- 100.44 = 2.754; k × ΔT0.44 = 0.048 × 2.754 = 0.1322. A = (3 ÷ 0.1322)1 ÷ 0.725 = 74.2 mil² (0.0478 mm²).
- Width = 74.2 ÷ 1.378 = 53.8 mil = 1.37 mm. Inside the board, with k = 0.024, 3.56 mm.
- At 35 °C the 1.37 mm × 35 µm trace is 19.0 mΩ over 50 mm: 57 mV of drop, 0.171 W of heat.
- The 1.0 mm trace already drawn is 54.3 mil². It carries 2.39 A at a 10 °C rise, and at 3 A it rises 16.7 °C; at 42 °C it is 26.7 mΩ, 80 mV and 0.240 W.
The calculator reports the 1.0 mm trace as 73 % of what is required and says so. It will not fail on the bench; a 42 °C trace is nothing to FR-4. In a sealed enclosure at 55 °C, next to a driver that is heating the board, and with the connector pins themselves rated at 3 A, it is the wrong place to spend the margin. Widen it to 1.4 mm or move the pins.
Checking a finished board
The design rise is a prediction, and the first assembled board is the test. Run it at its full load, in its enclosure if it has one, and look at it with a thermal camera: solder mask has an emissivity of about 0.9 and reads truthfully, bare copper and shiny solder do not, so put a piece of matt tape or a dab of matt paint on the spot to be measured. A trace that shows the rise you designed for, within a few degrees, confirms the copper and the assumptions; one that shows twice the rise usually means a via field or a thermal relief that is carrying the current through less copper than the drawing implied, or a trace that was etched narrower than drawn. A fine thermocouple under Kapton tape does the same job for a single point and is what to leave in during a long test.
Then do the test at the temperature the board will live at. A cabinet on a factory wall in Lahore in June is at 55 °C inside before anything is switched on, and a sealed box on a roof in Multan is hotter. A board that was tested on a bench at 25 °C and never in an oven or on that roof has not been tested; the enclosure takes away the convection the outer-layer curve assumed, and every part's rise stacks on an ambient that is 30 °C higher than the bench. The heat sink calculator does the same reasoning for the semiconductors on the board, whose case-to-ambient path is usually a bigger problem than the copper. Ahmedonics tests its own boards this way, in an oven at the site ambient, before a batch is built.
References
- IPC-2221B, Generic Standard on Printed Board Design, section 6.2 — conductor thickness and width for internal and external layers: the charts and their curve fit
- IPC-2152, Standard for Determining Current-Carrying Capacity in Printed Board Design, 2009 — measured data on real boards: planes, board thickness, enclosures, altitude
- IPC-6012, Qualification and Performance Specification for Rigid Printed Boards — minimum copper plating in plated holes and on surfaces by class
- Douglas Brooks and Johannes Adam, PCB Design Guide to Via and Trace Currents and Temperatures, Artech House, 2021 — the physics behind the charts, thermal simulation, via currents and the origin of the IPC-2221 data
- IPC-A-610, Acceptability of Electronic Assemblies — what a production assembly may and may not look like