# 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 Commented Feb 7, 2019 at 10:18
• Is the 50 amps continues or not? Commented Feb 7, 2019 at 10:18
• Yes its continues. According to online trace width calculator i would need about 50mm width which is huge
– razz
Commented Feb 7, 2019 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 Commented Feb 7, 2019 at 10:30
• Do you mean a high-current PCB bus for example?
– razz
Commented Feb 7, 2019 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: Note 1 mil = 0.001 inch

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
– razz
Commented Feb 7, 2019 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. Commented Feb 7, 2019 at 11:48
• Can you give me any example of a bus-bar that will fit perfect for my problem?
– razz
Commented Feb 7, 2019 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. Commented Feb 7, 2019 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
Commented Feb 7, 2019 at 14:38