3
\$\begingroup\$

I've been working on a light controller, GPS tracker, anti-theft, etc. board for my e-bike and I originally designed the 48V - 12V DC converter around a standard sixteenth-brick power converter (PS1):

Rusher 2.0.0

These sixteenth-brick power converters have been great for prototyping but they seem to run hot and consume more power than I would prefer when under no load.

So I used TI's WEBENCH Power Designer to build a circuit around the TPS54561 step-down DC-DC converter and this is what I've come up with:

Power Supply Schematic

Power Supply Prototype

This seems like it should work but I have some questions:

  1. Is there any technical reason why the example layout in the datasheet, the layout in Power Designer, and most other PCB examples I've found online don't use a ground fill/ground plane on the front layer? It seems to me that a larger ground plane will help with heat dissipation.
  2. Won't the thermal vias under U1 will wick away the solder paste from the exposed ground pad, should I be concerned about this? Tented vias do not seem to be an option at the price point I'm willing to pay (nor do they seem to be the correct solution). I've seen references to filling the vias with thermally conductive epoxy; is this something I should do? If so any gotchas to keep in mind?

These are all two layer boards with standard stackups from either Aisler or OSH Park and I'm using a modified T-962A infrared IC oven for the reflow (have been hand soldering up to this point so this power supply will be my first reflow).

Also moving the power supply off the main board to a dedicated PCB seems to make the most sense to me as that will allow me to make changes to either without rebuilding everything.

Update:

The original PCB was meant to be a prototype before I moved the power supply circuit onto the main board but since I've decided to keep this as a separate module I updated the design.

  • Switched to a smaller schottky diode
  • Increased the fill thermal trace width from 0.508mm to 0.6mm
  • Went with a complete ground fill on the top layer

Power Supply Module

\$\endgroup\$
7
  • 2
    \$\begingroup\$ It's not ideal to have vias on an exposed pad in volume manufacturing due to wicking, but for one off parts you can usually just put slightly more solder paste on the pad to compensate for wicking. Definitely use the smallest diameter vias your factory supports. \$\endgroup\$ Commented Oct 29, 2022 at 20:05
  • 2
    \$\begingroup\$ @jonathanjo It's a DOSA standard size/layout for DC-DC power converters sunpower-uk.com/glossary/power-brick \$\endgroup\$ Commented Oct 29, 2022 at 20:15
  • 1
    \$\begingroup\$ If you go for <=0.3mm vias, you normally don't have wicking. The diode for your buck looks quite large, why not take a smaller one and make the output loop smaller? Also you can move your input caps near to the TPS54561 to reduce the input loop size. Further, if you want to dissipate the heat better, directly connect your GND pins to the polygone pour. \$\endgroup\$ Commented Oct 29, 2022 at 20:23
  • 1
    \$\begingroup\$ Also have a look at the example land pattern and solder paste in the datasheet. \$\endgroup\$ Commented Oct 29, 2022 at 20:36
  • 1
    \$\begingroup\$ @HansPeterLoft thanks for the feedback. The vias are currently 0.4mm but both fabricators I use can go to 0.3mm so I'll shrink them. I was also thinking the diode was overkill but I used what Webench suggested. A quick search shows I could easily switch to something like VS-50WQ10FN-M3 and save a bunch of space. Can you clarify what you mean when you said "connect your GND pins to the polygone pour"? Are you talking about removing the thermal reliefs on ground pins? \$\endgroup\$ Commented Oct 29, 2022 at 20:42

1 Answer 1

1
\$\begingroup\$

Is there any technical reason why the example layout in the datasheet, the layout in Power Designer, and most other PCB examples I've found online don't use a ground fill/ground plane on the front layer? It seems to me that a larger ground plane will help with heat dissipation.

On a two layer board its generally harder to route with a ground fill, on most boards I've seen they don't do a fill on the top layer. Some RF boards require a fill on the top layer and connecting vias (many of those are 4 layer anyway).

Won't the thermal vias under U1 will wick away the solder paste from the exposed ground pad, should I be concerned about this? Tented vias do not seem to be an option at the price point I'm willing to pay (nor do they seem to be the correct solution). I've seen references to filling the vias with thermally conductive epoxy; is this something I should do? If so any gotchas to keep in mind?

Yes, they will wick away solder. It's usually not a huge problem with thermal pads, there generally is enough solder to fill most of the area underneath the chip. If this is a critcal application then you would probably need to fill it. If this is a one-off board you could extend the thermal solder pad and hit it with an solder iron and give it some extra flux. If this is a production board you'll probably want to fill the vias somehow. Another option would be to use vias with a small drill size OR even move some of the vias away from soldered side of the pad.

Also, the ground traces on the fill are very small in this area, they should be thicker. enter image description here

\$\endgroup\$
1
  • \$\begingroup\$ Thanks for the feedback. I updated the OP with a new PCB layout that has incorporated some of the feedback I've received here (including slightly larger thermal relief traces). \$\endgroup\$ Commented Oct 30, 2022 at 7:01

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.