August 23, 2026
“Is a 1 mm trace wide enough for 1 A?” This is a common PCB power-routing question, but it has no universally correct answer without defined operating conditions. A 1 mm trace made with 1 oz copper does not behave the same as one made with 2 oz copper. Its resistance, voltage drop, and temperature rise also change depending on whether it is on an external or internal layer and whether it is 10 mm or 100 mm long. PCB current-carrying capacity is therefore not a simple conversion between current and trace width. It is an electrical, thermal, and manufacturing problem.
Current flowing through copper generates Joule heating:
P = I²R
Trace resistance depends on the resistivity and geometry of the conductor:
R = ρL／(W × T)
Where:
A longer, narrower, or thinner trace will generally have higher resistance. Because heating increases with the square of current, a relatively small increase in current can cause a much larger increase in power dissipation.
The useful engineering question is therefore not simply, "How many amperes can this trace carry?" It is:
Under the expected ambient temperature and cooling conditions, are the trace temperature rise, voltage drop, and reliability still acceptable for the product?
IPC‑2152 approaches conductor sizing by relating the required current‑carrying capacity to an acceptable conductor temperature rise on the finished printed board. It does not provide one fixed width that applies to every PCB.
A fixed ratio omits the boundary conditions needed to evaluate a real design. At minimum, the following factors can change the result.
Copper weight is commonly expressed in ounces. For preliminary communication, 1 oz copper is often associated with a nominal thickness of approximately 35 μm. However, the design should ultimately use the finished copper thickness and manufacturing tolerance after etching and plating.
If the layout specification says only "1 oz" without distinguishing base copper from finished plated copper, the calculated conductor cross‑section may not match the fabricated board.
An external trace can exchange heat directly with the surrounding air, while an internal trace is enclosed by dielectric material. Their heat‑transfer paths are different.
Actual temperature rise also depends on nearby copper planes, dielectric spacing, board thickness, and overall copper distribution. A single internal‑versus‑external multiplier cannot represent every stackup.
A trace operating in a 25 °C room with an allowable 20 °C rise is not equivalent to the same trace inside a 70 °C enclosure.
The temperature limits of nearby components, laminate, connectors, solder joints, and the enclosure must also be considered. Heat from an adjacent power component may preheat the PCB and reduce the additional temperature rise available for the trace itself.
Two traces with identical width and copper thickness will have different resistance and voltage drop if their lengths differ.
In low‑voltage, high‑current power systems, voltage drop can affect the load voltage, regulator transient response, or measurement accuracy even when the trace temperature is still acceptable.
DC current, pulsed current, motor‑start current, and the RMS current in a switching converter should not be treated as interchangeable values.
A short current peak may not produce the same steady‑state temperature rise as continuous current, but the design still needs to consider pulse energy, transient copper temperature, connector capability, and fault current before protection devices operate.
A wide power trace does not guarantee that the complete current path has the same current‑carrying capability. Common bottlenecks include:
Via current capability cannot be determined from drill diameter alone. Finished hole size, barrel copper thickness, via count, arrangement, pad dimensions, and local thermal conditions all affect the result.
The review should therefore follow the complete current loop and identify its smallest conductor cross‑section and likely hot spots rather than measuring only the widest section of the main copper area.
Opening the solder mask and adding solder may reduce part of the DC resistance, but it should not be treated as a precise or repeatable substitute for copper cross‑section.
The thickness and shape of the solder deposit can vary with the process, and solder has a different resistivity from copper. If the rated current depends on achieving a particular solder volume, manufacturing consistency and long‑term reliability require separate validation.
More controllable options generally include:
Before selecting an approach, the designer should still confirm minimum spacing, etching capability, copper‑thickness uniformity, lamination structure, and cost implications with the PCB manufacturer.
| Check item | Information the RD should provide or confirm | Possible risk if omitted | | :--- | :--- | :--- | | Current conditions | Continuous, RMS, peak current, and duration | Underestimated heating or unnecessarily wide routing | | Environment | Maximum ambient temperature, airflow, and enclosure condition | Higher actual temperature rise | | Temperature‑rise target | Acceptable conductor temperature rise | No meaningful definition of "safe current" | | Finished copper | Base copper, plated copper, and tolerance | Smaller actual cross‑section than modelled | | Layer and stackup | Internal/external layer, nearby planes, and dielectric spacing | Thermal model does not match the board | | Trace geometry | Minimum width, length, neck‑downs, and transition areas | Local voltage drop or hot spots | | Via structure | Count, hole size, barrel copper, and arrangement | Overheating or reduced reliability at layer transitions | | Voltage drop | Maximum allowable drop at the load | Insufficient power‑rail margin | | Validation | Simulation, prototype measurements, and worst‑case testing | Problems discovered only during system validation |
Start by defining the maximum ambient temperature, allowable temperature rise, current waveform, voltage‑drop limit, and intended copper thickness. IPC‑2152 data or an appropriate thermal‑analysis tool can then be used to establish an initial conductor size.
After layout, review every neck‑down, pad, via transition, and nearby heat source. For high‑current products, high ambient temperatures, sealed enclosures, or high‑reliability applications, calculations should be treated as a starting point. Temperature rise and voltage drop should be measured on prototype boards under worst‑case operating conditions.
A Texas Instruments application report likewise explains that current‑carrying capability is linked to permissible temperature rise. Heat from nearby components can also make an estimate based only on trace self‑heating too optimistic.
There is no universally valid answer expressed as a fixed number of millimetres per ampere. Copper thickness, trace length, layer location, allowable temperature rise, environment, vias, and the complete current path must be evaluated together.
For R&D teams, the most effective approach is not to search for a more conservative rule of thumb. It is to define the electrical and thermal conditions before PCB release and ensure that the circuit, layout, and fabrication teams are working from the same assumptions.
For designs involving high current, heavy copper, parallel conductors across multiple layers, or specialised via structures, eCloud can help organise the fabrication conditions and DFM confirmation items before PCB prototyping, allowing the intended trace geometry and copper specification to be checked against practical manufacturing capability.
