15
\$\begingroup\$

I have some power traces (net VIN) in my PCB design that might (in an extreme scenario) carry up to 1A of current. Although nominally, I wouldn't expect to see more than 250 mA. These are 50 mil traces, just to be safe, and since I have to switch layers, I have put two 28 mil hole vias. Is it a bad idea to use double vias like this?

enter image description here enter image description here

\$\endgroup\$
2
  • 1
    \$\begingroup\$ Just a note that a 50mil track, external, 2oz copper has a resistance of 5.05mΩ/in. For 10°C temp rise, it is good for 4.7A. At 4.7A, it would drop 23.7mV/in (likely much thinner tracks can be used, unless very long.) \$\endgroup\$
    – rdtsc
    Jul 7 at 20:15
  • \$\begingroup\$ Thank you for the heads up. I probably oversized it too much. Since I don't expect very large currents (<1A), I wouldn't expect the voltage drop to reach 23 mV/in. But still, could've made it thinner. Thx. \$\endgroup\$ Jul 7 at 23:25
21
\$\begingroup\$

I use multiple vias to connect power traces to other layers all the time on many projects: -

enter image description here

Is it a bad idea to use double vias like this?

No, it's a valid way of doing it. Many of the connections in the picture above use 24 vias. Mind you, the tracks are carrying over one hundred amps and are multi-layer connected.

\$\endgroup\$
1
  • 3
    \$\begingroup\$ That's a great example, Andy! \$\endgroup\$
    – JYelton
    Jul 2 at 17:05
17
\$\begingroup\$

Not a bad idea. In fact it's recommended when you have high currents and you're changing layers as it reduces track impedance.

There are other considerations like whether to use a couple of large vias as you have, or multiple smaller vias. Ask your fabricator whether this is worth worrying about. Personally, I tend to use the same size via and place them at about 1mm pitch for stitching large current tracks or polygons.

If you have solid planes (ground or otherwise), you may want to try to space the vias in such a way that the planes have connectivity between the vias on the other layers. In other words, avoid creating a "slot" in the plane.

\$\endgroup\$

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.