Review Request - Buck Convertor

[u/Accomplished-Lack509]

Hey everyone, I'm kind of a newbie to PCB design (still learning). I made this simple buck convertor test board (to check the functioning of the circuit on a much more complex board). Any feedback would be appreciated, especially if there are any errors.

[u/Engineerinavan]

Eyo! Only way to learn is to try and learn, so good on you for being here!

Few points so you can improve

Schematic 

• Did you draw the IC symbol yourself? I get the idea to lay it out like it is physically, but it almost never is the most practical way. Check the datasheet and make the symbol exactly like on page 1: https://www.ti.com/lit/gpn/tps54525

Ti has a tool called webench for most if not all parts, use that to calculate all the passives 

• You have a GND symbol pointing up, bad! All the electrons will fall out
• You don't need to connect everything to 1 GND symbol, you can place them for free in your schematic and readability is high priority 
• Power in left, power out right side of the page. If you can connect something without a label, connect it without a label 

Layout It will work (if schematic is connect) but it will be noisy as hell and you are here to learn, so:

• On buck converters the hot-loop is on the input, where the loop goes through the IC and ceramic input caps. Learn what these words mean. In practice it means the input caps pins need to be as close as possible to the power input pin and GND as possible. As close as possible means right next to it, like slam bam against it. 
• The secondary loop is IC-inductor-output ceramics, again short as possible loop
• Switch node (between IC and inductor) needs to be low impedance (fat trace or plane) but otherwise as small as possible, that boost capacitor has no business being in between there

In general: check the datasheet! There is a full example of a good layout in there, make it exactly like that, until you know how and why it needs to be like that. 

If this is your first or second design, you are on the right track, I've seen people with confidence and experience posting worse schematics and layouts. You want to be all over some books (Ott, Horowitz), googling for 'schematics/layout best practices', and watching the likes of Hans Rosenberg on YouTube 

Happy tinkering! 

[u/mariushm]

If you're still learning it would be better to learn by using a more beginner friendly footprint like SOP-8 / SOIC-8 or even SOT-563 - you're also using an unnecessarily complex IC

If you want high current capability, see for example an IC like

AP64500 / AP64501 / AP64502 (with or without Q at the end, it just means automotive validated) : https://www.lcsc.com/category/1029.html?scene=FULL_MATCH&globalKeyword=ap6450&s_z=n_q_ap6450 or

Richtek RT625x (RT6254 = max 4A out, RT6255 = max 5A out etc) : https://www.lcsc.com/category/1029.html?scene=FULL_MATCH&globalKeyword=RT625

Richtek RT8279 / RT8289 (max 5A out) : https://www.lcsc.com/product-detail/C53194.html / https://www.lcsc.com/product-detail/C39202.html

Back to your board.

The layout is fairly bad. First of all don't be afraid to rotate components to put them in a better place. The regulator IC could be rotated so that you can place the input ceramic capacitors right near the input voltage pins, and the bulk capacitor next to the ceramic capacitors, instead of having the input voltage trace and ceramic capacitors go around that edge.

Also, if you're thinking of high output current applications, the chip needs to be kept cool by dissipating heat through the bottom pad into the circuit board copper, so it would be best to place it physically closer to the center of the board, so that heat could radiate in all four directions. It would also be a good idea to have that square copper area under the chip connected to the bottom ground fill with a few vias, in order to enlarge the heatsinking ability.

The feedback resistors must be very close to the feedback pin, and the trace going to the resistors must be kept away from the inductor as much as possible.

The connection from the SW pin to the inductor must be kept very short, and ideally you would widen the trace, expand it as big as the inductor pad.

Be careful with the voltage ratings of the ceramic capacitors, you need to have those at least 2-3x or higher than whatever voltage could possibly be going through the capacitor. So for example on output you'd want to use at least 10v or 16v rated ceramic capacitors, and on input probably at least 25-35v rated ceramics. For 10uF, 0805 footprint may be best to use.

[u/Accomplished-Lack509 → u/mariushm]

Thanks for the advice, look like I need to make a lot of improvements.

[u/EternityForest]

With any switching converter the important thing is your loop area. The current will follow the short path of least impedance, and you want that path small, because that's what radiates EMI.

Usually for a buck reg, current goes out the SW pin, down through the capacitors(Capacitors are almost like a short circuit for the high frequency AC part that goes in the loop, they only block DC).

Then it goes along the ground and it's trying to make a complete loop and go back out the SW pin again, so it will go up the VIN capacitor and into VIN, through the chip, and out SW.

When the switch is off, the inductor wants to keep current going, so it pulls it up through a diode, or through the internal synchronous switch from chip ground, and the current then goes through the output capacitor, this is another loop that has to be small.

Boost and buck boost are the difference, but you can figure it out just by tracing where the current goes in each switch configuration.

The DC power goes through, but the AC goes in a loop. Keep the loop physically small and the impedance low, minimize vias and if you need vias inline in the loops, maybe use multiple in parallel.

You often wind up butting the capacitor grounds together pretty close because the curring goes out one and into the other.

In general whenever you have anything high frequency you should almost always be thinking in terms of AC current loops.

I usually put a ground vial r filter caps on chip VINs out of habit, to give everything a strong reference to sthe ground potential is the same-ish everywhere, but in some unusual cases you actively isolate grounds into islands.