Grok Bot
PCB Trace Width: How to Size Traces for Current, Heat and Voltage
How to size PCB trace width for current: IPC-2221 formula, IPC-2152 guidance, a quick width table, copper thickness, inner vs outer layers and spacing.
Short answer: PCB trace width sets how much current a copper trace can carry before it heats up too much. The classic IPC-2221 formula gives about 0.30 mm (12 mil) per amp on a 1 oz outer layer for a 10 °C temperature rise, and wider for inner layers, thinner copper or a lower allowed rise. The newer IPC-2152 standard replaces the old charts with test data that also accounts for board thickness and nearby copper planes, and it’s the better reference for high current PCB design. Pick the width from current and allowed temperature rise first, then check voltage drop, impedance, spacing and your fabricator’s limits. AI design tools help by reading each part’s current from its datasheet and flagging every net whose trace is too narrow before fabrication.
Why PCB trace width matters
Every copper trace has resistance. When current flows, that resistance turns into heat and voltage drop. A trace that’s too narrow for its current runs hot, which can lift copper, darken the laminate, shift nearby component values and, in the worst case, act like a fuse. Even when it doesn’t fail, it drops voltage that your regulator or load never sees.
Too wide has a cost as well. Wide traces eat routing space, make dense boards harder to route and change the impedance of signal lines. The goal isn’t “as wide as possible”. It’s the right width for each net’s current, temperature budget and electrical role.
What sets PCB trace current capacity
Four things decide how much current a trace can carry:
- Cross-sectional area. Width times copper thickness. Double either one and you roughly double the copper available to carry current.
- Allowed temperature rise. A 10 °C rise over ambient is a common, conservative target. Allowing 20 °C or 30 °C permits a narrower trace, but the board then runs hotter.
- Layer position. Outer traces shed heat into the air. Inner traces are wrapped in laminate, which insulates them, so the old rules treat them as carrying about half the current for the same width.
- Surroundings. Board thickness, nearby copper planes and neighbouring hot traces all change how fast heat leaves the trace. This is exactly what the newer IPC-2152 data captures.
The IPC-2221 trace width formula
For decades, designers have used the formula in IPC-2221, derived from old charts:
I = k × ΔT^0.44 × A^0.725
Here I is current in amps, ΔT is temperature rise in °C, A is cross-sectional area in square mils, and k is 0.048 for outer layers or 0.024 for inner layers. To get width, solve for A and divide by the copper thickness: 1 oz copper is about 1.378 mil (35 µm) thick.
Most online trace width calculators use exactly this formula. The table below shows its results for a 10 °C rise:
| Current | 1 oz outer layer | 2 oz outer layer | 1 oz inner layer |
|---|---|---|---|
| 0.5 A | 0.12 mm (4.5 mil) | 0.06 mm (2.3 mil) | 0.30 mm (11.8 mil) |
| 1 A | 0.30 mm (11.8 mil) | 0.15 mm (5.9 mil) | 0.78 mm (30.8 mil) |
| 2 A | 0.78 mm (30.8 mil) | 0.39 mm (15.4 mil) | 2.03 mm (80 mil) |
| 3 A | 1.37 mm (53.8 mil) | 0.68 mm (26.9 mil) | 3.56 mm (140 mil) |
| 5 A | 2.77 mm (109 mil) | 1.38 mm (54.4 mil) | 7.19 mm (283 mil) |
Treat these as a starting point, not a guarantee. Fabricators also have a minimum trace width, often around 0.1 to 0.15 mm on standard processes, so very small calculated widths get rounded up anyway.
IPC-2152: the newer standard
IPC-2152, published in 2009, came from new thermal testing and replaces the IPC-2221 charts for current capacity. Its main lessons are practical:
- Inner traces aren’t always worse. The old rule of halving inner-layer current is often too conservative. With copper planes nearby, an inner trace can carry close to what an outer one does.
- The board matters. Thicker boards and boards with large copper planes spread heat better, so the same trace runs cooler.
- Planes are heat sinks. A plane close to a trace pulls heat away from it, which is one more reason to plan your stackup early.
If you’re doing high current PCB design, use a trace width calculator that supports IPC-2152, or your EDA tool’s built-in version, and enter your real board thickness and plane layout. The IPC-2221 numbers above remain a safe, conservative check.
Copper thickness: the other half of the equation
PCB trace thickness is set by copper weight. Standard boards use 1 oz copper (about 35 µm) on outer layers and often 0.5 oz or 1 oz on inner layers. Moving a power layer to 2 oz copper halves the width you need for the same current, which can be the only way to fit a power path through a crowded area.
Heavier copper isn’t free. It costs more, needs wider minimum spacing and etches less precisely, so fine-pitch parts on the same layer get harder. A common compromise is heavy copper on one or two power layers and standard copper everywhere else. Remember too that outer layers are plated, so their final thickness is usually a bit more than the base foil.
Beyond heat: voltage drop and impedance
A trace can be thermally fine and still too narrow. Check two more things:
- Voltage drop. A long 1 A trace at 0.3 mm on 1 oz copper has a resistance of roughly 1.6 mΩ per mm of length, so 100 mm drops about 0.16 V. For a 1.0 V processor core rail, that’s a serious error. Widen the trace, use a plane, or add remote sense.
- Impedance. For high-speed and RF signals, width is chosen for controlled impedance, not current. A 50 Ω microstrip has a fixed width for a given stackup, and you shouldn’t widen it just because you have room.
PCB trace spacing
Width and spacing go together. Spacing between conductors depends on the voltage between them, whether the traces are on an outer or inner layer, and whether the board is coated. IPC-2221 gives minimum clearance tables by voltage, and safety standards for mains-powered products often require more. For low-voltage digital signals, spacing is usually limited by crosstalk and the fabricator’s capability rather than by voltage. For mains, motor drives and high-voltage supplies, use the clearance and creepage values from the relevant safety standard, not just the PCB rule of thumb.
Practical rules for high current traces
- Size each power net from its real worst-case current, including startup and fault current, not the average.
- Use copper pours or planes for currents above a few amps instead of very wide traces.
- When a high current path changes layers, use several vias in parallel. A single small via can carry much less current than the traces it connects.
- Avoid necking a wide trace down to a narrow pad entry for a long distance. Short neck-downs are fine; long ones become hot spots.
- Keep high current paths short and away from sensitive analog circuits and precision references.
- Set net classes with minimum widths in your EDA tool so the DRC catches mistakes.
Common trace width mistakes
- Using one default width for every power net.
- Forgetting that inner layers often have thinner copper.
- Sizing for average current and ignoring peaks or motor stall current.
- Checking temperature but not voltage drop on low-voltage rails.
- Routing a power net through one via.
- Widening controlled-impedance traces to “be safe”.
Where AI helps
Trace width errors are easy to make because the current in each net isn’t written on the schematic. An AI design assistant can read each component’s current rating from its datasheet, estimate the worst-case current on every power net, and suggest a width per net class using IPC-2152 or IPC-2221 for your actual stackup and copper weights. It can flag traces and vias that are too small, long power paths with excessive voltage drop, and spacing that doesn’t meet the voltage between nets. During component selection, it can also point out when a part’s current pushes you toward heavier copper, so you can plan the stackup before layout starts.
FAQ
How wide should a PCB trace be for 1 amp?
Using IPC-2221 with a 10 °C rise, about 0.30 mm (12 mil) on a 1 oz outer layer and about 0.78 mm (31 mil) on a 1 oz inner layer. IPC-2152 may allow narrower inner traces when planes are nearby.
What is the difference between IPC-2221 and IPC-2152?
IPC-2221 is a general PCB design standard whose current charts date back decades. IPC-2152 is a dedicated current-capacity standard based on newer testing that accounts for board thickness, copper planes and layer position.
Does copper thickness change trace width?
Yes. Doubling copper from 1 oz to 2 oz roughly halves the width needed for the same current and temperature rise, at the cost of higher price and wider minimum spacing.
Are trace width calculators accurate?
They’re good starting points. Most use the IPC-2221 formula, which is conservative. For high current designs, use an IPC-2152-based calculator with your real stackup and confirm with thermal measurement on the prototype.
How does AI help choose PCB trace width?
AI can read component currents from datasheets, calculate the required width per net for your stackup, and flag narrow traces, undersized vias, voltage drop problems and spacing issues before fabrication.
Next step
Want every power net checked for the right trace width while you design? Talk to the IntelCAD team about AI-assisted PCB design and component selection for your next board.
Design your next board by describing it.
Start Your DesignRelated posts
1 min read
Thermal Vias and PCB Thermal Management: A Practical Guide to Sizing, Spacing and Via-in-Pad
Learn how thermal vias move heat through a PCB, how many to use, how to size and space them, when to use via-in-pad, and how to avoid solder wicking.
1 min read
PCB Ground Plane Design: A Practical Guide to Grounding, Return Paths and Stitching Vias
Learn how a PCB ground plane works, why return paths matter, when to split ground, how to place stitching vias and how to avoid ground bounce.
1 min read
Controlled Impedance PCB Design: A Practical Guide to Rules, Stackup and Testing
Learn when a PCB needs controlled impedance, how trace width and stackup set it, how to use an impedance calculator and how to specify it to your fab.