Sizing a trace on a PCB to carry 50 amps

Currently working on a 4 layer pcb-card where I need to trace for 50 amps, any ideas how I can design it?

Any tips would be appreciated. Thanks!

• try to use as wide traces as possible it's usually better than using more layers, due to less power density hence less local heating – Anton Ingemarson Feb 7 at 10:18
• Is the 50 amps continues or not? – Anton Ingemarson Feb 7 at 10:18
• Yes its continues. According to online trace width calculator i would need about 50mm width which is huge – Linus Jönsson Feb 7 at 10:22
• Have you thought about not directly carrying this current on a PCB? Sometimes it's better to use an additional, external piece of copper – Tom L. Feb 7 at 10:30
• Do you mean a high-current PCB bus for example? – Linus Jönsson Feb 7 at 10:34

Some work was done by years ago on this and the relevant standard is IPC2221

The basic concepts are as follows the thicker the copper the better, the wider the copper the better. Putting high current tracks on external layers is better as heat can escape easier.

That said for really high currents supplementing the tracks with external conductors helps. I have left an area free of solder resist for this and soldered of copper braid (e.g. solder-wick) in the past for home or low volume products. For higher volumes I have used copper bus-bars.

That said the maths

Let $$\I\$$ be the track current $$\[\text{amp}]\$$
Let $$\A\$$ be the cross-sectional area if the track $$\[\text{mil}^2]\$$
Let $$\T\$$ be the allowable track temperature rise $$\[\text{ }^oC]\$$
Let $$\W\$$ be the required track width $$\[\text{mil}]\$$
Let $$\M\$$ be the mass of copper on the PCB $$\ [\text{oz} / \text{ft}^2]\$$
Let $$\k\$$, $$\b\$$ and $$\c\$$ be constants defined by the IPC standard.

$$\ A = \dfrac{I}{(k \cdot T^b)^{1/c}}\$$

Then, the Width is calculated:

$$\ W = \dfrac{A}{M \cdot 1.378} \$$

where k, b, and c are constants resulting from curve fitting to the IPC-2221 curves

For IPC-2221 internal layers: $$\k = 0.024\$$, $$\b = 0.44\$$, $$\c = 0.725\$$

For IPC-2221 external layers: $$\k = 0.048\$$, $$\b = 0.44\$$, $$\c = 0.725\$$

If you do not feel like doing the the maths yourself there are many online tools

Assuming 2oz copper, 10C rise I would go with some kind of bus-bar as track is of the order of 1.3 inch wide.

• Thanks for answer, I understand the calculations but my problem still exist. Lets say I use 2 oz thickness and 50 amps at 60C ambient Temperature with 20 temp rise.Trace width will then be about 22mm on external layer(top layer) which is still huge. I need to solve this somehow – Linus Jönsson Feb 7 at 11:41
• You can get 4oz copper from many PCB vendors, solder links (or copper braid) in parallel with the track or use both sides of the board. – Warren Hill Feb 7 at 11:48
• Can you give me any example of a bus-bar that will fit perfect for my problem? – Linus Jönsson Feb 7 at 11:57
• @LinusJönsson Recommendations for specific products are off-topic for this site. This answer has given what you asked, which was how to size the trace. – Elliot Alderson Feb 7 at 12:39
• @LinusJönsson if 2 oz or 70 µm thickness and 22 mm track width is not what you like, you may use 140 µm and 12 mm or 210 µm and 8 mm. But you can't get a solution with 35 µm and less than 5 mm track width made with unobtainium superconductive plating. – Uwe Feb 7 at 14:38