I'm making an ESP32 board to control some 12V outputs, so I got an LM2675-3.3 buck converter IC (datasheet) to power the MCU. This is my first time designing and soldering a PCB and I'm guessing I may have done a bad job with either the soldering or with the converter layout. I've already burned through 3 ICs, although one by misplacement. One worked correctly only after I accidentally grounded the on/off pin (datasheet says it can float), but it seemed to have a slight drift and a day later it dropped from 3.3 to 2.6 inexplicably. The last one was soldered very carefully on an empty board and it also didn't output anything until I fiddled with the on/off pin, and even then it was something below 1V.

Before I order a new batch, can anyone tell me if there are any glaring mistakes in the layout? The whole board is two layered, full back ground plane except around an ADC chip. The converter section on the PCB Schematic

  • 1
    \$\begingroup\$ Any particular reason why everything is so spread out? Have you looked at page 25 of the datasheet for layout suggestions? \$\endgroup\$
    – winny
    Commented Jun 19 at 11:52
  • 1
    \$\begingroup\$ Switching regulator -> loop inductance puts gravel in your machinery. It's nice that you have a ground plane, so your starting condition is good, but you want your design as tight as your EMS allows you to place the components in the switch loop, so IC1, C10, C9, U1 and L1. \$\endgroup\$
    – winny
    Commented Jun 19 at 12:01
  • 1
    \$\begingroup\$ After the converter you're routing a bunch of traces and even what look like bypass capacitors over a cut in the ground plane which is bad practice. Try not to break the ground plane if you can, and if you do avoid routing traces over the cut since the return currents will not be able to follow the trace back to the converter. \$\endgroup\$ Commented Jun 19 at 12:09
  • 1
    \$\begingroup\$ Your layout is far too spread out. Too much parasitic inductance. The line between U2 and C10 is especially bad, but really all of it could stand to be tightened up. Switching converter datasheets always have layout recommendations; I highly suggest you take a look at that and try to follow those guidelines. You don't have to replicate the layout exactly, but pay attention to the guidelines. \$\endgroup\$
    – Hearth
    Commented Jun 19 at 14:52
  • 1
    \$\begingroup\$ Carefully inspect and reflow all solder joints, especially for the IC and passive components. Ensure you are using low ESR capacitors as recommended in the datasheet. \$\endgroup\$
    – liaifat85
    Commented Jun 19 at 14:54

1 Answer 1


Your feedback pin is not connected in the right way, take a look at the typical application from the datasheet:

typ app


Maybe you could salvage your pcb if you bend the fb pin up and run a little wire to the positive end of C9

  • \$\begingroup\$ Oh, I completely missed this, wow. Thank you for the suggestion, I'm gonna go try it, it's definitely worth the ESP32 I already soldered. \$\endgroup\$
    – Axl Vang
    Commented Jun 19 at 12:02

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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