help with buck regulator pcb

[apraxophobia]

I don't have much power electronics experience... And made a PCB using a design from TI's WebBench for a 12V to 6.5V, 15A regulator with an LM5117. I get the basic idea and I can more-or-less reason through how it works, but I am lost.

The output is correct (6.5V) and can drive small loads (I haven't tested large loads yet) but the noise is terrible. Clearly the switching is irregular and not at a fixed frequency. I've probed about every part of the board, and that irregular switching and noise is everywhere.

I was fairly careful during layout to adhere to the datasheet's guidelines but I did miss a few suggestions. That said, I didn't make any huge mistakes, and I'd be surprised if the layout is so severely wrong as to be causing this issue.

I know this is probably hard to fix, but even more broadly: How do I go about figuring out what the issue is? I've exhausted all the testing/probing I can think of. I need to get a design working ASAP. The webbench designs should be pretty good normally, right?

[T3sl4co1l]

There's no (or almost no) designators on the PCB, could you bring those forward a bit?

What I'm guessing is Rsense, has almost no grounding; there's tons of vias under the controller, but not here?  Maybe other ground spots too.  But I'll take a look later when it's easier to review (see above).

Tim

[apraxophobia]

Sorry about that- attached is proper schematic and better layout photos with designators. Some of the larger input/output caps don't have designators but should be clear.

Vias under the IC were recommended by the datasheet/came with the footprint I downloaded.

[Whales]

How are you measuring the noise?  How much noise?

 - I assume you're hooking up a x10 scope probe directly on the output of the power supply. 
 - Make sure that the ground lead is also hooked up on the output, not somewhere else or disconnected.
 - Is the noise from the upstream power supply?  Try measuring just that with your board disconnected or disabled.
 - What is the noise floor of your scope?  My old 90's DSO is particularly bad.  Try measuring something else that you suspect is good as a control.

> Clearly the switching is irregular and not at a fixed frequency.

Fixed frequency operation is often only guaranteed for a range of loads.  At no-load you will often see pulse-skipping which adds a whole bunch of nasty lower frequency switching noise.  Attaching a load to the output may fix this.

[Someone]

I was fairly careful during layout to adhere to the datasheet's guidelines but I did miss a few suggestions. That said, I didn't make any huge mistakes, and I'd be surprised if the layout is so severely wrong as to be causing this issue.

Why not follow the example layout in the datasheet? You've lost all its embedded knowledge.

T3sl4co1l found a problem pretty much immediately, whether that is enough to salvage the design remains unknown.

[T3sl4co1l]

Some more documentation deficiencies:

And some layout comments. I think. Again, can only guess at what/where a lot of components are.



Spend time studying the datasheet/appnote layout -- appnotes in general are poor, but they're at least a starting point to go from.  Keep in mind that distance, trance length, body length, all count against you in terms of stray inductance.  You *will* see switching noise everywhere, because everything is coupled into the main switching loop: long grounds to few (mostly single!) vias means lots of nH's add up (figure ballpark 0.5nH/mm).  Use wide connections, lots of vias, especially when stitching top side to GND.

Maybe some ceramic caps on the output would be desirable too, I don't know.

The mostly solid bottom ground plane will help greatly with common mode, but do try to avoid trace length there, and when unavoidable, try to space traces so that ground can fill between them (and further, pour top side with GND and stitch that over the gaps made by bottom-side traces).  R29/C46 is especially egregious in this regard, crossing under the main switch node itself (I think), and thus preventing that node from having solid uninterrupted ground under it.

Tim

[apraxophobia]

What I am hearing is I do indeed need to be much more careful about layout!!

Thanks very much for all your suggestions- T3sl4co1l especially! Back to the drawing board I guess...

[tooki]

I don't have much power electronics experience... And made a PCB using a design from TI's WebBench for a 12V to 6.5V, 15A regulator with an LM5117. I get the basic idea and I can more-or-less reason through how it works, but I am lost.

The output is correct (6.5V) and can drive small loads (I haven't tested large loads yet) but the noise is terrible. Clearly the switching is irregular and not at a fixed frequency. I've probed about every part of the board, and that irregular switching and noise is everywhere.

I was fairly careful during layout to adhere to the datasheet's guidelines but I did miss a few suggestions. That said, I didn't make any huge mistakes, and I'd be surprised if the layout is so severely wrong as to be causing this issue.

I know this is probably hard to fix, but even more broadly: How do I go about figuring out what the issue is? I've exhausted all the testing/probing I can think of. I need to get a design working ASAP. The webbench designs should be pretty good normally, right?

When you say “based on”, do you mean you used the WEBENCH schematic and component values, or did you also use its PCB layout? While they aren’t always perfect (especially if you manually change components to ones in other packages) but they’re a great place to start. If you didn’t use their layout, why not?

Alternatively, what about the layouts in evaluation boards or reference designs? These often give great insight (often explained in the documentation) on how to design a real board.

[AnalogTodd]

One major thing I would do with your layout as well is look at grounding. You have 15A switching on this board! This is not trivial!

I see right away that your sense resistor in series with the low side FET goes through a tiny trace to a single via to your ground plane. This is going to completely throw off your current sensing.

A switcher like this takes careful thought to lay out, especially considering the spikes of current you will get. Layout must be done while thinking of parasitic inductance in every single trace and then comparing that to what the current waveforms look like. High dI/dt with fast edges is impossible with too much parasitic inductance.

[Sagar]

Barely I can found any Ground return paths, keep the switching circuit away from signal paths and try to add more different value capacitor at input. TI always provide referecne PCB design, if you go with that it works perfectly. btw, did you get the PCB and soldered everything, an you share noise behaviour.