DC-DC Converter Layout Review

[kaevee]

Hi,

I need a onboard DC-DC converter for a project.

The DC-DC converter is available in SOT-23-6 package. I have created the circuit based on example from manufacturers datasheet. The layout is based on manufacturers recommendations as there was no example layout.

How do I improve this layout?

Venkat

[Rerouter]

Feedback trace is crazy long and inductive, don't understand why its on a separate layer,

Archive the project into a zip file and it seems quite easy to package up nicely

main goal is shrinking the loop area as much as possible.

[palpurul]

The most import part of a syncrounous buck (or just plain buck) converter design is the input capacitor placement.
You have to connect both capacitor pins with the shortest traces possible to the IC pins. From the picture I don't really understand where the ground and voltage "pours" are. You don't seem to have any. I don't even understand how the ground pins of input capacitors and IC are connected together. I assume they got connected in the ground plane underneath, but I am not really sure.

[kaevee]

Feedback trace is crazy long and inductive, don't understand why its on a separate layer,

Can I have the feedback trace on top layer?

I have attached the project archive (Kicad).

The most import part of a syncrounous buck (or just plain buck) converter design is the input capacitor placement.
You have to connect both capacitor pins with the shortest traces possible to the IC pins. From the picture I don't really understand where the ground and voltage "pours" are. You don't seem to have any. I don't even understand how the ground pins of input capacitors and IC are connected together. I assume they got connected in the ground plane underneath, but I am not really sure.

You are right. I had missed out traces for input capacitors. I have drawn the traces for input capacitors.

[palpurul]

I don't think input capacitor placement is great.
I would connect the grounds(IC's PGND and input cap ground) at the same layer not through vias at the ground plane underneath. If possible don't use thermal relief.

[T3sl4co1l]

The vias don't need to be in dense clusters.  A few is enough to ensure a low resistance, low inductance connection.

Prioritize them by placing them closer to component pads.  One beside each bypass capacitor, and one inbetween them.  One for the reg ground pin.

Feedback path doesn't really matter, but the layout can be made smaller by pulling everything together.

Switching loop is entirely within the regulator, which appears to be either a synchronous or integrated diode type.  All that's needed is a bypass cap close between its VCC and GND pins.

You may find it's worthwhile putting a pour on the switching node, and surrounding the inductor's pad.  This allows the inductor to dissipate more heat into the board.  (You already have this on the output side.)

Everywhere else, pour GND on both layers.  Not really anything that needs to be stitched in this design, just the added copper will improve heat dissipation.

Leave a gap between the inductor pads, so the ground can pour between both sides.

Tim

[Rerouter]

Smallest loop area I can come up with in a short period of time,

The goals I used as a rough guide

- Keep switching node as small as possible to reduce external noise
- No signal traces under the inductor
- The switching current return path as short as possible (grounds tied together on the same layer)
- No ground under the inductor to prevent shorted turn heating
- Feedback taken after the output capacitors for the best regulation
- Keeping the load ground path connecting to its capacitor before heading back to the input, to help smooth out any load spikes
- Shortest path to the decoupling capacitors
- Shortest path on the feedback network (capacitor and resistor postions could be flipped, but does not change much,

Thing that I'm not 100% happy with is that ground loop near the feedback network, however I doubt it will cause much issues.

[kaevee]

Smallest loop area I can come up with in a short period of time,

Thanks for the layout. It looks very good and there is a lot to learn for someone like me.

I will build up this keeping the guidelines you noted.

Venkat

[asmi]

Feedback trace is crazy long and inductive,

That is irrelevant, especially inductive part, because feedback signal is rather slow.

don't understand why its on a separate layer,

Now THAT is a good thing if you can use internal layers to shield it from noisy nodes.

[asmi]

Thanks for the layout. It looks very good and there is a lot to learn for someone like me.

That layout is utter crap because it's very hard to assemble and impossible to rework.

[Rerouter]

asmi, do you want to suggest a better alternative then? I have the files open, and willing to respin.

There is 0.6mm or more between all components, you would need some very crappy tweezers to not be able to rework that

[asmi]

asmi, do you want to suggest a better alternative then? I have the files open, and willing to respin.

There is 0.6mm or more between all components, you would need some very crappy tweezers to not be able to rework that

Feedback resistors R1 and R2 are most likely to be replaced (to tune output voltage), so it's best to place them such that you can get to them with an iron (since it's not realistic to expect that a person asking help with DC-DC layout to own a tweezer soldering station, and even with them I think inductor will make accessing them very hard). Feedback trace needs to be as far away from noisy nodes (VIN, SW) as possible, it's best if it's shielded from them by internal ground layer(s). Also it's best to avoid routing traces under SMD caps and resistors because they increase chances of creating a short during reflow. Judging by the package, it's not a very high current converter, and so proper layout doesn't matter a whole lot (unless you need to minimize Vout ripple), but I think it's important to do things right from the get go.

[kaevee]

asmi, do you want to suggest a better alternative then? I have the files open, and willing to respin.

There is 0.6mm or more between all components, you would need some very crappy tweezers to not be able to rework that

Feedback resistors R1 and R2 are most likely to be replaced (to tune output voltage), so it's best to place them such that you can get to them with an iron (since it's not realistic to expect that a person asking help with DC-DC layout to own a tweezer soldering station, and even with them I think inductor will make accessing them very hard).

You are absolutely right. This is my first attempt to spin my own dc-dc converter. In fact, my first board since my school days! I did not share the information as I did not want reviewers to factor in my skills, experience and equipment in their feedback. I wanted a brutal and honest review from people with real life experience.

I do have a professional soldering and hot air station with tweezers and a decent microscope.

Venkat

[kaevee]

To OP:

In power electronics we have a concept called hot loop, which is the loop between decoupling capacitor and half bridge.

In a buck (step-down) topology, the hot loop is from the anode of the input cap to the high side FET (usually integrated in IC), to the low side FET (also integrated), to the cathode of input cap.

So, minimizing loop area between the CAP+/IC VIN/IC GND/CAP- is crucial.

As for output inductor and capacitor, it kinda doesn't matter that much.

For a boost converter it is exactly reversed -- output path is crucial, input is relaxed.

Thank you very much for this tips. There are certain things we can't learn from reading alone.

What will be the impact if one flips the input capacitors? Probably not relevant for this layout.

[kaevee]

What will be the impact if one flips the input capacitors? Probably not relevant for this layout.

Do you mean to rotate by 90 degrees or to place it under the PCB?

I meant under the PCB?