0
\$\begingroup\$

I have buck-boost converter using a TPS630250(4.2 ->Vin) - (3.3 -> Vout) in my PCB. This buck-boost converter can draw max 4A in buck mode and max 2A in boost mode.

While there is no load or there is light load ~150mA) in my PCB , My converter nicely keeps working. When I try to draw about 1A from LEDs (that I can not draw current), I am hearing sound from my inductor. Also, Output voltage of converter decreases to about 2.8V.

I sure from my soldering. I sure current from capacity of my power cable.

I am sharing with you my schematic and related datasheets. I wonder your comments and advice.Schematic of Voltage converter

My inductor datasheet : https://cdn.ozdisan.com/ETicaret_Dosya/516756_635936.pdf

My converter datasheet : https://www.ti.com/lit/ds/symlink/tps630250.pdf?HQS=dis-dk-null-digikeymode-dsf-pf-null-wwe&ts=1621014133772

layout with gnd polygon

layout without gnd polygon

\$\endgroup\$
9
  • \$\begingroup\$ Did you follow the layout guidelines in the IC datasheet exactly? Maybe you should show us your PCB layout. \$\endgroup\$ May 14, 2021 at 17:56
  • \$\begingroup\$ Could you provide a data sheet for your load? \$\endgroup\$ May 14, 2021 at 18:04
  • \$\begingroup\$ @SpehroPefhany I added part of voltage converter. \$\endgroup\$
    – fafeyto
    May 14, 2021 at 18:06
  • 1
    \$\begingroup\$ Your layout is not good! You have a very long trace for the PGND connection and your small signal ground connection is in series with the PGND trace which means the feedback circuitry is modulated by PGND. Not good for a switcher. The data sheet has a recommended layout and you should follow it for good reasons. \$\endgroup\$
    – qrk
    May 14, 2021 at 18:15
  • 1
    \$\begingroup\$ Note that capacitors can also make sounds, so you could try touching them with a small plastic or wood stick to hear if there is any change. \$\endgroup\$ May 14, 2021 at 18:30

1 Answer 1

5
\$\begingroup\$

I think you've shot yourself in the foot with your layout. You've got a high-power package, and three of your highest-current traces are long and thin.

When a switching supply IC vendor gives you a recommended layout, they mean it. Power ground, L1 and L2 are all high-current pins -- that's why the package has the unusually long stripes under there.

Note that in the recommended layout (shown below) they've maximized the area of the ground plane going to the power ground pin, and they've put vias under the chip package to get the L1 and L2 traces out to great big wide traces on the opposite side of the board.

Note, too, that they're bringing the input power out to a fill -- this is probably for thermal as well as electronic reasons.

You need to think like an electron -- and a phonon -- and make sure that there's plenty of copper for them to travel in the vicinity of that chip. If you can't follow the reasoning for their layout, then just copy it exactly.

enter image description here

(And the sound from the coil -- or possibly nearby caps -- is because voltages and/or currents are changing rapidly, making components bend or expand and contract. It's probably happening more than it should -- I would not be at all surprised if the deficiencies in layout were causing the circuit to oscillate, which would make any current/voltage excursions worse than normal).

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.