Electronics > Projects, Designs, and Technical Stuff

Question on buck converter layout

(1/3) > >>

thinkfat:
Hi,

I'm integrating a buck converter based on the TI LMR14030SDDAR into an adapter board for a GPSDO. I've attached the layout (top side only) and schematics here. I'm always scratching my head about the return currents, I think I've got it tight enough here, hopefully. The other head-scratcher is about the "cold" side of L201, for mechanical reasons there's a pretty large gap between L201 and the filter caps C206/C207, do you think this should be improved? The copper fill is pretty beefy, but I could duplicate it on the bottom layer and stitch it together with vias to reduce the impedance.

Output of the converter is 5.5V, around 2.2A peak, input will be 12V nominal. Switching frequency is set to 1MHz.

T3sl4co1l:
Looks good. :-+

(Edit: also, I'm assuming the bottom side, or inner layer, has solid ground pour.)

(I tend to be verbose on explanations or critiques, so take this as high praise ... or at least a pat-on-the-back for following the appnote, which, I didn't look up this one specifically, but they usually show something very similar to this.  It's pretty good. :) )

I will note just two things and an optional third:
1. You may want an LC at the input there, to keep sharp edges out of the input cable.  You have the flanking bypass caps which is great, but they still have some ESL which lets through some of the switching edge.  The buck input side is a noisy place, because the current is fully switched, 100% on to off -- you might have, oh Idunno, 60dB of attenuation there (a factor of a thousand), but out of a ballpark 10V step, that's still enough mV to pick up on a nearby radio.

Typical would be just a 0.1 to 1uH inductor in series, and probably just one more of those ceramic caps at the connector.

Optional 3: you may want a TVS here, to prevent overvoltage, and maybe also a series diode to prevent reverse polarity.  The problem is this: you plug in a DC adapter that's already charged to nominal 12V or whatever, and an inrush surge flows through the cable.  The cable has maybe 1uH of inductance, so there is a series RLC circuit between the supply's bypass cap (something fairly large, 100s uF), the cable inductance and resistance, and your ceramic bypass caps (and their ESR).  The fatality is this: the ceramic caps' capacitance drops sharply at high voltages, so instead of kicking to a peak of less than about 24V (as a linear capacitor would do: a film or electrolytic), the peak voltage can be 30, or 50 or even 100V, and that can easily damage the regulator.

So, just a SMAJ15A in parallel with the filter caps by the regulator, would be simple insurance for that.  And for series polarity protection, a PMEG3020 or B130 or ES1B or whatever would be fine, or a P-ch FET if you need low voltage drop.

2. The diode is pretty huge -- 5A, but you're only using 2 of it.  This saves a bit on conduction losses (although not really all that much, because the diode Vf curve is exponential), but likely will cost more on switching loss -- the 100s of pF (or is that into the nF, I forget) junction capacitance has to be charged with every cycle, and it adds up.

So, simply to say -- you may find higher efficiency with a smaller diode.  And if you don't have high operating temps, don't be afraid of a relatively leaky diode (like the aforementioned PMEG family), they tend to have lower Vf.

(Still higher efficiency can be had from a synchronous type regulator.  TI makes one that delivers 3A from a mere SOT-23!)

Okay, so maybe I got verbose as usual, anyway. :P

Cheers!
Tim

Siwastaja:
You can still move the diode a bit closer. It's likely more than good enough as it is, but I tend to place the components as close as possible within the manufacturing tolerances (of course respecting the courtyards and component-to-component body clearances), because such dense SMD board would likely be reflow soldered, and won't be manually modified in any case, so extra space is of little practical use. Moving the silkscreen designators "outside" the dense area, in one blob where the texts are approximately rotated and placed like the components, helps.

Note that the inrush voltage peak issue Tim mentioned can be also solved by adding a lossy standard aluminium electrolytic capacitor at the input, so that its capacitance is at least twice-three times the capacitance of the ceramics in parallel with it. This helps dampen any ringing you get if you add an LC filter, so good for EMI, too.

Agree on using a smaller diode.

capt bullshot:
In general, I second what Tim wrote, especially the part about protecting the input from plug-in overvoltage events. Looks like there's plenty of space left to add a nice large electrolytic paralleled to the input node, and some EMI suppression inductance in series.

Having a "longer wire" at the cold side of the inductor doesn't do much harm at all, its inductance just adds to the inductors value. It's a stable voltage node, and current ripple is relative harmless here EMI wise.
Go for small loops at these places first: Input capacitor + to switch input and input capacitor - to diode anode, and keep  the switching node as small as possible.
I'd further place the bootstrap cap closer to the switching node and try to elimitate that trace on the bottom side.
Edit: minize the total switching node area, e.g. I wouldn't flood fill a rather large with sw node potential.

thinkfat:
Thank you all for the input, I really appreciate it.

Regarding the suggestions:

The diode was chosen for a higher step-down ratio and current, I guess I can replace it with something like a SS33, or going for a smaller footprint, SK33SMB or maybe even SKL33. I guess I will decide by leakage current, because as I said, it's for a GPSDO, it will be a pretty warm environment.

About the bootstrap capacitor - I was following TI's layout recommendations who are trying to keep the ground loop on the top layer as tight as possible and they probably decided that it's better to break the bottom ground fill rather than cutting off the input caps from the switcher ground on the top layer. I do realize that I am kind of obstructing the ground loop on the top layer with the bootstrap cap, TI recommends a 0603 or smaller footprint here but I hope I can get away with 0805 because that's what I have in my parts bin ;) I stitched the ground side of the output input caps to the ground fill to amend. Now, if the path to the diode anode is more critical than to the switcher ground, I can move the bootstrap trace elsewhere on the bottom layer and put some vias around the anode, too. But I think it's probably going to be OK as it is.

Regarding minimizing the switching node area - good idea, I'll shuffle L201 around a bit and tighten up the copper fill.

Regarding the density of the board - I usually try to make the layout as tight as possible, too, but I will have to assemble them. I have to make amends for that ;)

Voltage spike created by inrush current - ok, I'll think of something here. Leaning towards a TVS diode, actually.

EMI suppression - I hoped that the input caps would take care of that. But I'll add an inductor here.

Another question - should I move C205 over to the other side?

Navigation

[0] Message Index

[#] Next page

There was an error while thanking
Thanking...
Go to full version
Powered by SMFPacks Advanced Attachments Uploader Mod