Can I get a small review about my buck converter?

I used to solder those mini pcb buckconverters with castellated holes from aliexpress to my PCB designs. It simply saved me some trouble and costs for most of my thru hole designs. And for ~50 cents and 4 whole pads to solder it is a good trade imo.

I am changing some designs to SMD and I would prefer to simply make my own buck converter as that is easier with SMT assembly.

I find it really hard to find the right IC for this. Besides the point that JLCPCB’s website is horribly in finding anything, there are soo many buck converter chips.

I eventually chose the MT2499A because it is A). the design does not use those huge aluminum capacitors which JLCPCB does not have in their basic component list. And B). there is no need for a Schottky diode…

I made a symbol and copied the schematic of the datasheet.


(N.B. the 88k7 resistor is not in the basic part list :smiling_face_with_tear: )
L =

Made the components

image
(dont min’d the wrong inductor 3D model)

backside

This particular thing is to supply an MG90 servo motor and an attiny. But in general I would like this circuit to supply 2A without problems.

Are there any pointers to this design?

Also, did I take a decent chip or should I use a different one for a reason??
My 2nd choise is the TPS543. This one is in the basic part list, but requires ~200uF capacitor…

Kind regards,

Bas

GND zones are an important part of an SMPS circuit and you’ve turned it off in your screenshot, which makes a review more difficult. Uploading the project itself makes it a lot easier. It looks like you’ve got thermal reliefs on the GND pad, which is not good. You want to use the GND zone as a heatsink, and this also means adding more thermal via’s.

R5 and C1 appear to share a common GND track. This is not good. It means that current spikes though the capacitor will shift the voltage feedback sense circuit. Separate those GND tracks from each other.

C1 also has a much bigger problem. Pad7 is only an enable pin, while all the current (spikes) go to pad 2. This means you have to put C1 very close to pad 2, while the track length to pad 7 is not critical.

You write you chose the MT2499A, but the schematic is missing the “2” in the device name.

What current rating? Those tracks look way too thin

Way too much stray inductance on the VCC and the bootstrap.

Is pin9 really connected to GND?

Check your capacitor values and/or footprints. All have the same package and footprint but C2 is 22nF and C1,3 & 4 are 22µF.

I would add a 0.1µf in parallel with C1 and C4. They would be for high frequency filtering and is usually the type of thing one would find in the development of a product. I believe you are expecting this to work the first round.

Power traces are needlessly thin. I would make them much wider.

I would try to get C3 and C4 much closer to Pins 4 & 9. This is the path of the switching currents and the loop should be as small as possible.

Be aware there are other parts with the same Partnumber MP2499A #2

I thought it was funny to find these “proprietary…” words:
image
on a datasheet which is posted on the open internet.

and

Yes that part looks like it could also work.

C2 is the bootstrap capacitor. IT IS CONNECTED WORNG!!

It should be connected between the BS and SW pins. (I am not familiar with this chip, but a bootstrap capacitor is a standard requirement on buck ICs which have an Nchannel high side MOSFET, whether that MOSFET is internal or external.)

And yes, particularly for the output capacitors, use big fat copper zones; not thin traces. Copper on a pcb is free (once you have bought the unetched board) so use it. Proper layout (including generous use of copper zones) will help make the layout as good as it can be.

1 Like

You can use the kicad E-series calculator to find a replacement.

In this case it seems like you can put a 150k and a 220k in parallel with only a half percent error (which is is probably okay, considering the usual tolerances, but it also shows you more exact solutions if required).

1 Like

Net-(L1-Pad1) is far to thin (stray inductance a.t.l.). In a SMPS the switched side of the inductor should be as thick as possible. Maybe add a copper zone instead of the track?

Like so:

kicad_2KNeg1IEoA

The zone is not completely filled as I just put a footprint in there for demo, without any schematic and nets.

C1 is the most critical part, you have to place it right! :slight_smile:
in the sense that you must move it from the left to right, place it closest to Vin(2)/gnd(4) pins.
fb resistors are placed ok.
as others has said, use thick copper areas in the high current path.

But then the trace from output to R4 is far too close to the switched inductor side. Ok, this is a buck converter, so switching noise is not terribly strong, but anyways.
I would put it further away or to the other side.

My comment was really a caution to be sure the OP didn’t pick a different MP2499A that JLCPCB was stocking.

Oddly enough, I’ve seen “CONFIDENTIAL” on a number of datasheets on line. Seems to mean nothing to some MFG. Or they didn’t bother to remove the CONFIDENTIAL when the document was released to the public.

First I noticed is that C2 connection is surprising, but I see it was already told.
If I were designing that PCB:

  • I would certainly rotate L 90° left to get the switching net as small as possible.
  • I would not route feedback track so close to switching net.

For DCDC converters I always look for two current paths for two DCDC states:

  • one is from C1 through pin2 to pin3 and then through L to C3 and back through GND to C1.
  • second is from pin 4+9 to pin3 and then through L to C3 and back to pin 4+9.

I imagine that they are alternately lit and my task is to make a distance from PCB that you can’t notice flashing as short as possible.

Thanks for the feedback all.

Yeah I noticed. I changed it after my post.

All have the same package and footprint but C2 is 22nF and C1,3 & 4 are 22µF.

Yeah. I used different ones now, the ones in the order of micro are now 0603, the nano order ones are 0402. The feedback resistors were also a little large. Those are now 0603 though I guess 0402 would suffice as well.

I tried to implement all feedback. And I think I have a better pcb now.

  • I added more vias close to the groundplane underneath the chip. I also drew 1mm traces to remove the thermal reliefs.
  • I used 0.5mm trace for all high current traces. (2A is my aim)
  • I rearranged the position of components to keep traces as short as possible.
  • I added 2x 100nF capacitors.
  • There are no traces underneath the inductor.


(pardon me, C5 silktext must be rotated 180 degrees)

This traces on the back is the VCC trace. I was not sure where to put it exactly. I kept it is as short as possible.

I added the schematic and the board files.
servoDriverMicroswitch.kicad_pcb (359.3 KB)

servoDriverMicroswitch.kicad_sch (100.9 KB)

Kind regards,

Bas

Pay attention that as BobZ was telling, the connection of the boost caps is wrong, must be between pin 3 and inductor!

Boost = C2 || C5 at last schematic.

I see now. I will change it

EDIT:
changed it.

Perhaps move the U1 refdes away from the C6 pad?

I see several suggestions for making traces “as fat as possible” - they should be big enough to carry the necessary current, but not much bigger, otherwise you get increased capacitive coupling (especially on the switch node).
Also, the feedback signal should be kept away from any non-dc traces as much as possible to avoid noise coupling over.

1 Like