Heat in a multilayer PCB comes from two sources. One is the power dissipated by chips and power devices themselves. The other is the resistive loss generated as current passes through copper foil and vias. The second source is often underestimated, yet in power loops, power modules and heavy-copper windings, much of the temperature rise comes from the I²R loss of the conductor itself. Copper layers in a multilayer PCB do two jobs at once: they carry the current and they move heat out to the board surface and copper pours. Current carrying and thermal design are the same problem in this part of the board.
Undersized copper shows its effects only after power is applied. A trace that is too narrow heats up as current rises, pushing temperature rise beyond the limit and accelerating insulation ageing, or melting the foil open in a severe case. Spacing that is too tight invites creeping discharge and breakdown in high-voltage or humid conditions.
Inner layers sit buried in the substrate and dissipate heat poorly, so at the same width they carry roughly 10% to 20% less current than outer layers; sizing inner traces from outer-layer figures leads to excessive rise once the board runs. Transient surge current is more damaging still, because the weakest point of the foil has no time to shed heat and its temperature spikes to the melting point of copper in a short interval. A current-carrying review and a drawing check before production catch all of these; correcting them after the boards are built costs far more.
The temperature rise of a multilayer PCB follows from copper weight, trace width, the allowed rise, the layer the trace sits on, and how vias and planes are connected. Copper weight sets the base current capacity, width scales it in proportion, the chosen rise decides how much current a given cross-section can carry, and the cooling difference between outer and inner layers revises that figure again.
Copper weight and trace width set the current capacity of a multilayer PCB
General-purpose boards most often use 1 oz copper, about 35 µm thick. High-current boards commonly use 2 oz at about 70 µm, moving up to 3 oz at about 105 µm and 4 oz at about 140 µm for heavier loads, with 6 oz and above reaching 210 µm and more. Doubling the copper weight roughly doubles the current capacity at a fixed width. Measured data bears this out: a 2.8 mm wide outer trace carries about 8 A at a 20 ℃ rise, roughly 10.8 A at 40 ℃, about 16 A at 100 ℃, with an ultimate sustained current near 20 A.
Outer and inner layers do not end up with the same copper thickness. Inner traces keep the base copper value because they are etched and then pressed directly into the stack. Outer traces are drilled after etching and receive a full-board electroless copper deposit, adding roughly 25 to 35 µm, so a 35 µm base foil finishes at about 52.5 to 70 µm on the surface. Trace width carries its own manufacturing tolerance, typically +10 µm to −60 µm between the designed and etched value, and chemical residue at corners makes those spots the weakest point. Calculating the current capacity of a trace with a turn calls for a reduction factor applied to the straight-run figure.

The chosen temperature rise changes trace width estimation in a multilayer PCB
The classic empirical relation in IPC-2221 links current to a 0.44 power of the temperature rise and a 0.725 power of the cross-sectional area. That structure carries two lessons. Doubling the allowed rise raises the current capacity of a given width by only about 1.36 times, so buying capacity with a higher rise is inefficient. Doubling the cross-section raises capacity by about 1.65 times, which makes widening or thickening the copper the more effective move. The table values in the newer IPC-2152 track real boards more closely and are the better basis for a production release.
A 10 ℃ rise is the common choice that balances safety against space. With 1 oz copper on an outer layer, a 1 mm wide trace at a 10 ℃ rise carries about 1 A; 2 oz under the same conditions carries about 2 A. Inner layers cool less effectively and carry roughly 10% to 20% less at the same width, so their traces need to be wider. Common practice runs like this: consumer digital boards may use 10 to 20 ℃, with main power rails kept near 10 ℃; power boards, automotive, industrial and medical boards hold the rise to 10 ℃; battery charge and discharge paths stay at 10 ℃ to avoid swelling at high temperature. The calculated width also needs 20% to 30% of margin, so the routed trace ends up roughly one to two tenths wider than the raw figure.
Cooling differences between layers decide copper allocation in a multilayer PCB
FR-4 has a thermal conductivity around 0.3 W/(m·K), while copper sits near 385 to 400 W/(m·K), a gap of more than a thousand times. Outer traces touch the air directly and cool readily. Inner traces are wrapped in substrate, so their heat has to travel sideways along the foil to a via or the board edge, and the same cross-section carries visibly less current. Putting high-current loops on outer layers is the most direct cooling measure in a multilayer PCB; where space runs out, an inner layer can be turned into a solid copper pour so several layers share the current.
The temperature rise alone does not tell the whole story. Conductor temperature equals ambient plus the rise, so a 10 ℃ increase inside a 60 ℃ enclosure gives 70 ℃ at the trace, still a safe value. With a hotter ambient, the same rise can approach the glass transition temperature of the laminate. Near or above that point the substrate may warp and blister, the bond between foil and substrate weakens, and a deformed trace can crack. Thick and high-layer-count boards have longer heat paths and need more margin here.
Spacing has to be reviewed alongside current. Ordinary low-voltage signal traces usually need 0.2 mm or more. Any path tied to power input or mains voltage needs creepage allowance set by the working voltage; a 230 V mains input calls for at least 1.5 mm between traces, with an isolation slot or removed solder mask where needed to meet the withstand requirement. Humid, dusty or high-altitude environments shorten the effective spacing, and boards for those conditions need a wider figure again.
How power and ground planes affect current and heat in a multilayer PCB
Inner power and ground planes in a multilayer PCB do more than supply and return current. They are also a large cross-section for current and a broad surface for heat. A continuous copper plane has low impedance, spreads current evenly and keeps local current density down, which holds heating down. Once a plane is cut into fragments by routing, current detours, density climbs at the narrow necks and those spots become hot. Power and ground layers should stay as intact as possible; where a split is unavoidable, keep its boundary away from high-current paths and tie same-potential copper with vias.
High-power or high-current applications can parallel several power planes to spread current and reduce voltage drop. When copper layers are added, the connection bridges and vias have to be paralleled as well, or the bottleneck simply moves to the bridge. Calculations show that adding ring copper while keeping a single-layer bridge leaves loop resistance unchanged, because the limit sits at the bridge. Decoupling capacitors belong close to the power pins of the device, shortening the charge path and reducing supply noise at the same time.
Via current capacity sets the layer-to-layer connection of a multilayer PCB
A plated through hole connects layers through its barrel. Barrel copper thickness stays much the same across one board, so the current capacity of different hole sizes depends mainly on barrel circumference. Common test coupons cover 0.15, 0.25, 0.3, 0.5 and 0.7 mm drills, and a larger hole gives a longer circumference and more capacity. Via design cannot rest on drill diameter alone; the copper area it actually reaches and the surrounding cooling matter too, and figures from an ideal test coupon do not transfer directly to a populated, densely routed board.
Transient surge current is especially hard on vias. A steady current settles into a stable rise that can be read from a table. A transient surge leaves the barrel close to adiabatic for a short interval, driving temperature up sharply until the thinnest point melts. When several vias carry current in parallel, position and symmetry decide the split, and an unbalanced layout overloads part of the array first. Sizing power-loop vias to the peak current with adequate margin is more dependable than drawing them to an average value.
Heavy copper and skin depth shape high-frequency current in a multilayer PCB
At direct current, thicker copper always carries more. At high frequency that relation stops holding. Skin depth can be estimated as 66 divided by the square root of frequency in millimetres, giving about 0.21 mm at 100 kHz and about 0.09 mm at 500 kHz. Copper beyond the skin depth carries little current and adds proximity effect, which raises AC loss. High-frequency high-current windings such as planar transformer coils usually use several thinner copper layers in parallel, preserving the cross-section while holding down AC loss.
A 300 W class design illustrates the point. Eight layers of 4 oz copper in parallel serve a 200 to 700 kHz operating range; 4 oz is about 0.14 mm, close to the skin depth at 200 kHz and beyond it above 500 kHz, so capacity comes from the number of parallel layers, with each layer held near the skin depth. A heavy-copper stack also has to be checked for height, since every added layer eats into core window or assembly clearance. Meeting the DC resistance target does not settle the temperature rise; current sharing across layers, proximity effect and local hotspots all need confirmation on real samples.
Checkpoints for current carrying in a multilayer PCB
- Set copper weight from the highest operating current and allowed rise, moving to 2 oz or more for high current and favoring outer layers over inner ones.
- Estimate trace width from IPC-2152 tables or the empirical rule, then add roughly one to two tenths of margin; widen inner traces beyond the outer-layer figure.
- Use a 10 ℃ rise, keep main power rails and battery paths at that figure, reserve higher rises for space-constrained signal runs, and recalculate conductor temperature when the enclosure ambient is high.
- Open the solder mask over high-current traces and plate them, run several traces in parallel, or use a solid inner pour to spread the load across a wider area.
- Keep power and ground planes continuous, route split boundaries away from high-current paths, and connect same-potential copper with vias.
- Size vias from peak current and barrel circumference, keep parallel vias symmetric, and make sure the bridge is not the limiting part.
- For high-frequency high current, choose copper thickness against skin depth and use parallel thin layers to preserve the cross-section, checking the stack height as well.
- Set spacing from the working voltage and environment, keeping at least 1.5 mm for mains paths and widening it further for humid or high-altitude use.
Multilayer PCB current carrying questions
How much current does a 1 oz, 1 mm trace carry? On an outer layer with 1 oz copper at about 35 µm and a 10 ℃ rise, a 1 mm trace carries roughly 1 A. Inner layers cool less effectively and carry about 10% to 20% less at the same width, so they need to be wider. Production designs should still be checked against the standard tables or a current-carrying simulation.
How can current capacity be estimated without a standard table? Start with the rule of thumb: about 1 A per millimetre of width on 1 oz outer copper and about 2 A on 2 oz, scaling roughly with copper weight. Relaxing the rise from 10 ℃ to 20 ℃ adds only about three tenths to capacity, so widening or thickening the copper pays off better than allowing more heat.
Does thicker copper always carry high-frequency current better? It holds at direct current and not at high frequency. Copper beyond the skin depth adds little capacity and increases proximity effect. High-frequency high current favors several thinner copper layers in parallel, which preserve total cross-section while keeping AC loss in check.
Current carrying in a multilayer PCB follows a set order: fix copper weight and trace width from the highest current and allowed rise, revise inner-layer figures for their poorer cooling, then check power planes, vias and skin depth, and finally review spacing against voltage and environment. Doing this before routing is frozen keeps current and temperature problems out of the first powered prototype.



