Buck converter feedback from power plane?

[HwAoRrDk]

I'm designing a PCB that includes a buck converter. It will be on a 4 layer board with layers of signal, ground, power, signal, where the output of the buck converter is supplied into the power plane.

Would it be appropriate to have connection to the VOUT for the feedback voltage divider simply take VOUT straight from the power plane? That is, it taps straight down to the power plane right next to the upper resistor of the feedback voltage divider rather than running a distinct trace directly to the output capacitors?

Attached image is of the layout as I have it at the moment, showing the top layer and inner power plane layer. Circled upper-right is the feedback via to the power plane; bottom-left is the output from the buck converter.

P.S. Any other critique of the layout also welcome. The buck converter is a TPS565201, or perhaps an AP62400.

[moffy]

The distances are close and the power plane should be low impedance, I personally cannot see a problem with picking the feedback from the power plane.

[Faranight]

Route the feedback trace away from sources of noise such as the inductor or the switching input.
Tap the feedback trace directly beneath or close to the output capacitor (away from the inductor).

[HwAoRrDk]

Yes, I'm aware of the conventional practices for routing the feedback, as mentioned above. I know what one would normally do.

But as I was going to need to route the trace on the bottom layer of the board, I questioned myself what the difference was between that and just picking it up from the power plane.

There is a ground plane between the power plane and the switching node, so even though the inductor and switcher are kind of located between the point of delivery of VOUT to the power plane and FB pickup, surely there will no adverse effect?

[Terry Bites]

https://techweb.rohm.com/product/power-ic/dcdc/dcdc-design/4682/

[Faranight]

The switcher needs a very responsive feedback loop to compensate for any power fluctuations. If your power plane happens to have stray inductance in-between the buck output and the feedback tap
 then you may end up with unwanted oscillations. The vast majority of buck converter datasheets and application notes recommend the feedback loop be "kelvined" directly to the output caps that are close to the switcher IC.

[moffy]

For what it's worth, I agree with the OP, the distances on the plane are small, and the plane has plenty of copper between the output and the feedback point, I think the drop would be negligible. But if in doubt, you can do it both ways and use a 0R link to select between one or the other and you can test it.

[Phoenix]

It might work fine, but why risk it when there are simple optimisations. I will identify that the switching current return path from the output caps to the input caps is directly the same line as the proposed voltage feedback path... Doesn't sound so good.

I would suggest a small rearrangement where the enable signal is on bottom layer allowing the feedback signal to connect directly from the left side of the output caps to the voltage divider (flip the top feedback resistor 180).

[tooki]

I'm designing a PCB that includes a buck converter. It will be on a 4 layer board with layers of signal, ground, power, signal, where the output of the buck converter is supplied into the power plane.

Would it be appropriate to have connection to the VOUT for the feedback voltage divider simply take VOUT straight from the power plane? That is, it taps straight down to the power plane right next to the upper resistor of the feedback voltage divider rather than running a distinct trace directly to the output capacitors?

Attached image is of the layout as I have it at the moment, showing the top layer and inner power plane layer. Circled upper-right is the feedback via to the power plane; bottom-left is the output from the buck converter.

P.S. Any other critique of the layout also welcome. The buck converter is a TPS565201, or perhaps an AP62400.

The datasheet explicitly says to use Kelvin connections for both the Vout and ground connections to the feedback divider. We have (at least) three sample layouts provided: the datasheet, the eval board, and the Webench Power Designer layout. (And the note https://www.ti.com/lit/an/slva922/slva922.pdf explains how they developed the eval board layout.) Not all actually implement the Kelvin ground connection, but what they all do is give the Vout feedback trace a wide berth around the inductor.

I would definitely, as a rule, give the EN input trace lowest priority when routing DC-DC converters.