I have a curious problem which I have been trying to solve for a few days now and I just can not understand what is going on.

I have designed a SMPS which takes 24V input and outputs 5V (which is then further down regulated to 3V3, and 1V8 for circuitry). The IC I am using is a LT3680, and the schematic is below this post.

I have this circuit on a 4 layer PCB with proper grounding and heat dissipation features and it works like a treat - no problem whatsoever. I also have this exact same circuit on a homemade single layer PCB with very poor grounding and crap layout. This is a PCB I put together in a few hours just to test some things out.

I apply 24V through a relay to the SMPS circuit on the crappy homemade PCB and the regulator IC IMMEDIATELY pops with a loud bang and it blows a hole in its package. I apply 24V through the same relay, but jump it to the well designed PCB with the regulator, and then jump the 5V output back to the crappy PCB with other (3V3, 1V8) linear regulators. I switch the relay to apply power and everything works well. I tried it hundreds of times without issues. I desolder the LT3680 IC from the well designed PCB, and solder to the crappy PCB (or take a new IC from the box), apply power, and it blows immediately. (I desoldered the known-to-be working ICs just to eliminate the possibility of a bad batch of ICs).

Basically, LT3680 blows up every time on the homemade PCB, and works under the same conditions on the well designed PCB. I have compared the schematics of the boards and there are NO differences in the SMPS circuit (I have designed both of them). The only difference that I can see is PCB layout (very crappy compared to very well designed as suggested by the datasheet).

The question is could poor layout (in particular poor grounding), cause such SMPS IC failure (and why)? Or should I keep investigating, although I am desperate at this point as there seem to be no differences between the boards and the conditions I use them except in layout.


EDIT2: Added both sheets of the schematic Sheet Two: enter image description here

Sheet One: enter image description here

EDIT: Added layouts of the two boards

Crappy Board Layout (U201 is the SMPS IC): enter image description here

Good Board Layout (note this is a 4 layer board with GND plane): enter image description here

  • 1
    \$\begingroup\$ Are you sure the two circuits are the same (i.e. no shorts/opens where there shouldn't be any?) Use a multimeter to check continuity between different nodes. \$\endgroup\$ Oct 30, 2014 at 21:13
  • 1
    \$\begingroup\$ Also, actually seeing the layout in question would help. \$\endgroup\$
    – W5VO
    Oct 30, 2014 at 21:15
  • \$\begingroup\$ @helloworld922 I'm pretty sure the two layouts are the same. \$\endgroup\$
    – IgorEE
    Oct 30, 2014 at 21:30
  • 1
    \$\begingroup\$ Poor layout could definitely be destructive. Could be due to ringing on the switch node going higher than the abs max rating, or below the max negative voltage allowable. (Of course this goes for any other pin, but the switch node is a good place to start looking.) \$\endgroup\$
    – John D
    Oct 30, 2014 at 21:41
  • 1
    \$\begingroup\$ @JohnD I thought so as well, and I have looked at the o-scope traces in single shot mode to see what happens when the relay switches to apply power. It does overshoot and ring for a short while, but never goes over 36V which is allowable for the IC. This is with the setup on the well designed board. I never looked at this on the crappy board, so it might be it. The well designed board also has a 30V zener, the crappy one does not which might be preventing overvoltage on the good board but not on the crappy one. I blew all my LT3680s for the time being so can't test until I get some more. \$\endgroup\$
    – IgorEE
    Oct 30, 2014 at 21:45

1 Answer 1


All the example circuits in the LT3680 datasheet show at least a 4.7uF capacitor directly between Vin and Ground. Your circuit appears to have nothing.

Since your 'protection' diode prevents current from flowing back into the supply, there is nothing to soak up voltage spikes on Vin except for the IC itself. Combine that with the extra inductance of long thin traces, and... boom!

  • \$\begingroup\$ Yeah, this. No input capacitance at all = Bad idea! \$\endgroup\$ Oct 31, 2014 at 7:32
  • 1
    \$\begingroup\$ Hi Bruce, you might be right, although I have just over 10uF of capacitance. I have added the first sheet of the schematic of the crappy PCB at the top. As you can see c101 (10uF) and c102 (100nF) are across the supply and GND. As these capacitors are before diode D201, not directly between LT3680 VIN and GND, do you still believe your answer is valid? \$\endgroup\$
    – IgorEE
    Oct 31, 2014 at 8:05
  • 1
    \$\begingroup\$ The diode isolates your capacitors from the IC - positive voltage spikes won't go through diode because it is reverse biased when the voltage at Vin is higher than Vcc. You should put 4.7uF electrolytic capacitor directly across the IC. \$\endgroup\$ Oct 31, 2014 at 8:52
  • \$\begingroup\$ Reading through the datasheet a few more times and having a good think about it I think you are right and this is the reason for the IC failure. I will verify as soon as I obtain more LT3680 ICs, but I am accepting this as the answer. Thank you for your help! \$\endgroup\$
    – IgorEE
    Nov 1, 2014 at 12:34

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.