1
\$\begingroup\$

I'm needing to design a PCB for power distribution. I have a 90W (5V 18A) power supply that will be responsible for powering 5 USB Type A outputs, each USB drawing up to 12.5W (5V 2.5A) MAX.

I'm used to PCB layout for low power digital electronics but this will be the first time designing something drawing this much current.

Am I just able to use a top layer polygon pour for 5V, and then the bottom layer polygon pour for ground? Or is there a reason I should have a thick trace (2oZ copper(?), thick width(?), solder on top of trace(?)) with each USB drawing off a main rail (like in the digram below) Power Distribution

I'm just trying to workout whether to trace or polygon pour to ensure my PCB can handle up a potential of up to 12.5A draw.

Thanks

\$\endgroup\$
1
  • 1
    \$\begingroup\$ Looking at your topology, you may want to consider that the current is not equal in each segment. The current will be highest near the source. But as the main trace passes each drop point, there is less and less current. \$\endgroup\$
    – mkeith
    May 26 at 8:00
4
\$\begingroup\$

Copper pours should work fine. You can estimate the resistance of a track with an online tool, for a pour it works the same. Make sure it is not cut too much by tracks which would reduce its width.

If your USB connectors are surface mount, you will need vias to connect your USB's to the bottom layer and these have resistance too. So you need to check the copper plating thickness in the vias from your pcb fab. It's not pure copper, rather copper deposited by electroplating in a bath, so it has higher resistance. Check this calculator.

Also if a short develops at the end of a 5V 2A USB cable, or worse a 5V 500mA cable, it may not draw enough current to trip the 18A current limit in the supply. In this case the short will produce a lot of heat, which could melt the insulation, or start a fire. If the short occurs inside the device side USB connector of the cable it will heat up and melt or ruin the device's connector.

So it would be a good idea to add a 2A current limit for each outlet. There are USB power distribution chips that provide this functionality. A cheaper option is to use a polyswitch (PTC self resettable fuse) on each output.

\$\endgroup\$
2
  • \$\begingroup\$ This is really helpful I appreciate it. I'll definitely be taking your advice. The PTC is a good idea however if the USB connector is supplying power to a Raspberry Pi 3B+ which contains a fuse on it to prevent anything greater than 2.6A being drawn, with this information would you not bother putting a PTC fuse on the PCB or would you still add it? \$\endgroup\$
    – Explorex
    May 27 at 6:17
  • \$\begingroup\$ Yeah, because the fuse is there to protect the cable and connector which are not rated for 18A \$\endgroup\$
    – bobflux
    May 27 at 7:29
0
\$\begingroup\$

More copper is generally better, so pouring power on one side and ground on the other makes a lot of sense.

Be aware that the plating on vias is typically thinner than on the outer layers; if there’s a pin soldered into a hole there’s no problem but normal vias need to be large and numerous to carry significant current.

If you make slots in the solder resist you can reinforce the copper with solder, it’s not as good a conductor but it’s easy to deposit a thick layer.

\$\endgroup\$
4
  • \$\begingroup\$ I believe copper is about 6x more conductive. So to double the conductivity, the solder buildup needs to be 6x as thick as the copper. Another option is to solder copper bus bar to the PCB. \$\endgroup\$
    – mkeith
    May 26 at 17:00
  • 1
    \$\begingroup\$ 70 micron copper multiplied by 6 is 420 micron or 0.42mm so a 0.5mm bead of solder would more or less double the conductivity, a 1mm bead would be better still. \$\endgroup\$
    – Frog
    May 27 at 11:08
  • \$\begingroup\$ 140 um copper is also somewhat available, depending on what else is on this PCB. \$\endgroup\$
    – mkeith
    May 27 at 16:46
  • 1
    \$\begingroup\$ True, and many PCB houses can plate thicker than that, but at the expense of increased track/gap geometry. Larger vias are needed to allow effective through-hole plating. \$\endgroup\$
    – Frog
    May 27 at 20:08

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.