3
\$\begingroup\$

I am using a couple of SMPSs (MPM3610) on a 4 or 6 layer PCB. The recommended PCB layout seems to use solid copper regions to connect the design together.

Should thermal-reliefs be used on the capacitors and resistors? Does it have any effect on performance of a SMPS circuit?

On multi-layer boards, should unused layers underneath the power circuit remain empty, GND filled, or it doesn't matter?

Recommended PCB layout

\$\endgroup\$
  • \$\begingroup\$ Since you don't see them in the example layout, you probably don't want thermal relief on the large-bodied capacitors. Resistors probably won't be of much concern due to their lower current. The "Bottom Layer" image could be split up to have the FB trace on any non-noisy layer. Using more ground around the supply is a good plan, but does not necessarily preclude using lower layers for (non-sensitive) routing. \$\endgroup\$ – user2943160 Jul 6 '16 at 22:58
3
\$\begingroup\$

The large bodied capacitors should indeed avoid thermal relief unless absolutely necessary for manufacturability -- extra parasitics are not a good idea, and you will notice that the reference layout does not include them either. Thermals on the resistors are indeed a non-concern in this case, though -- their function is a low-current/low-noise one, and the extra resistance is insignificant compared to the resistors themselves.

The "Bottom Layer" on the reference board should be placed immediately adjacent to the top layer in your design -- this minimizes loop area and keeps outside traces from being coupled to. Other vacant inner layers under the DC/DC layout can be used for further thermal mass, while the bottom can be used for heatsink area. The feedback trace can go on any layer other than the top -- the reason why it isn't on top is to limit coupling to other critical nodes.

\$\endgroup\$
4
\$\begingroup\$

I had a field applications engineer from Linear Tech come by and review my SMPS layout and he definitely recommended I remove all the thermal reliefs on the input and output capacitors because they add inductance and degrade the performance.

It is small but does significant contribution. And there really is no need for thermal relief since your board is probably not hand soldered. Even if it were, the copper area on input and output are usually not so large as to be a problem.

You can leave thermal reliefs on the inductor (if you had an external inductor), resistors and small signal capacitors.

Layout is very critical with SMPS designs to prevent false triggering and subharmonic oscillation. Hope that helps.

\$\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.