1
\$\begingroup\$

I am designing a buck converter, based on a TI chip. Both the datasheet and an excellent document "Five steps to a great PCB layout for a step-down converter" show vias in the exposed pad, under the IC.

The application note states:

Starting with ground, vias are best placed directly under the IC so that the exposed thermal pad conducts its heat down into the PCB layers. This is required to achieve the IC’s best thermal performance.

And the example layout looks like:

Figure 6 from application note, the finished PCB layout and routing

Via-in-pad is an expensive service from most PCB manufacturers, especially at low volume. The design I hope to achieve will occasionally (but not continuously) run at the top of the converters capability at 5V / 8A (40W).

How important are these vias for thermal performance, and are there any ways to compensate for the lack of via-in-pad?

\$\endgroup\$
6
  • 3
    \$\begingroup\$ I use in-pad vias in most of my PCBs. I use JLCPCB and order 5-10 boards at a time and the shipping (to US) is always the most costly part of the order. \$\endgroup\$
    – earl
    Aug 18, 2023 at 16:32
  • 3
    \$\begingroup\$ "Via in pad" refers to a process involving drilling and plating a hole, then filling it with conductive epoxy, plating its surface, and polishing it flat to ensure even a small (e.g. 0.2 mm BGA) pin will adhere properly. In your case, with a pad nearly nine times bigger, you can almost certainly still make a good electrical connection even if the via is not filled and plated. My assembly house doesn't charge extra for QFN thermal via in pad; they just cap the via with solder mask to prevent capillary wicking. \$\endgroup\$
    – Matt S
    Aug 18, 2023 at 17:12
  • \$\begingroup\$ QFN via-in-pads can (and do, and perhaps even should) wick a little solder. This is probably a duplicate question but the answer is so simple (don't worry about it) it hardly warrants searching. Cheers! \$\endgroup\$ Aug 18, 2023 at 17:26
  • \$\begingroup\$ Perhaps I am misunderstanding @earl but adding plugged vias (to enable soldering to a pad) adds at least $50 to an order on JLCPCB. Do you plug the vias? \$\endgroup\$
    – David
    Aug 18, 2023 at 18:55
  • 1
    \$\begingroup\$ @David Simply design your board with vias where you want, and upload it to JLCPCB. If you have any questions, the online chat support is actually very good with these guys. And as Matt pointed out, your design does not require plugged vias and IMO most designs don't. Just use normal vias. \$\endgroup\$
    – earl
    Aug 18, 2023 at 18:57

1 Answer 1

1
\$\begingroup\$

I designed this board with four vias, which was the closest I could get within JLCPCB's design rules. This is a four layer board with an inner ground layer.

The important things I learned were:

  1. It's possible to have vias in pads - as per comments from earl and Matt.
  2. Poured planes help to radiate heat.

The final design looked like:

Segment of a printed circuit board from KiCad software

I could not directly compare with / without vias due to cost, but I did some thermal testing to check maximum temperature rise at ~55% load. I tested with a 50W 2R2 resistor as a dummy load, drawing approx. 2.2A / 11W at 5V. Every 15 minutes I checked temperatures using a thermal camera.

Thermal image of the PCB

The top copper zone for power output is clearly visible in the thermal photo, with the cut out underneath the inductor. The hotspot on the right is the controller chip (only 3mm x 3mm) and the hotspot on the left is the output connector.

I also logged temperatures for an hour. The controller chip peaked at 37°C (about 18°C above ambient). This is comfortably within the maximum ratings of the parts involved, and shows that closely following the recommended design is a sensible way forward.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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