11
\$\begingroup\$

I recently designed my first PCB, which houses LED driver circuitry for some custom lighting. I fastidiously followed the driver's datasheet (Diodes Inc AL8862QSP-13) in designing the circuit: making sure the inductor, capacitor, current sense resistor, and freewheel diode were suitable, and particularly ensuring input and output voltages (48v and 18-25v, respectively) were within spec.

I plugged it in and the LEDs lit briefly before tripping the power supply's overcurrent protection. I should have stopped here to think, but I instead connected it to a larger power supply (same voltage). Pop! All three drivers went up in smoke.

I've carefully reread the driver datasheet and scrutinized my design, and I am completely at a loss what might be wrong. My circuit is laid out exactly like the typical circuit in the datasheet.

The drivers are supposed to have overcurrent protection, so I'm not sure how they would have immediately blown up like that. This is only my second time doing SMD soldering (and I did it in a toaster oven), so that's a possible failure point, but the fact that 3 out of 3 drivers failed makes me think it's something other than that. Unless I possibly overheated the ICs in the toaster oven? I've also realized the exposed pad (EP) should be connected to ground, whereas I had it floating, but I don't think that's a major problem.

Can anyone provide suggestions? I've included a screenshot showing the schematic, pictures of the final product, and the KiCad PCB design (note that copper pours are not shown to make it easier to see the tracks). Inductor is 330uH (Bourns PM5022-331M-RC); capacitor is 10uF (Samsung CL31B106KBHNNNE); resistor is 100mOhm (Stackpole CSRN2512FTR100); freewheel diode is SMC DSS15U.

I have verified that the wire connections from J1 to the LEDs are in the correct order.

Track width was based on IPC-2152, which indicates that TINY (0.06mm) traces are sufficient for 40C rise with copper pour and 1oz copper. For safety, I increased this to 0.5mm. This board is also actively cooled with a fan. I've checked and double-checked to ensure the components are oriented properly.

Schematic for one driver

Images of board showing exploded driver

Screenshot of KiCad PCB design

\$\endgroup\$
5
  • \$\begingroup\$ Conversation in the comments has been moved to chat for further discussion. \$\endgroup\$
    – Null
    Jul 7 at 20:44
  • 1
    \$\begingroup\$ I don't think this is your only problem, but if you look at almost any buck converter the inputs and outputs are connected to planes rather than wires. In fact there may be almost no traces at all, only planes connecting components. Consider splitting the top layer into an input and output voltage plane separated by the converters while making the bottom layer a ground plane. You can route any control signals through traces on the top layer between converters. \$\endgroup\$ Jul 7 at 21:23
  • 1
    \$\begingroup\$ I didn't show it in the PCB diagram, but each side of the board is a plane - front is VIN, and back is GND. It would be impossible to do this for the LED power connections as there are 5 LED channels and this is only a 2-layer board. \$\endgroup\$
    – Reid
    Jul 7 at 21:29
  • \$\begingroup\$ It is not impossible if you improve your layout. Rather than a single plane for vin, move the converters so they span the middle of the board and make half of the layer vin and half of it vout. Leave ground on the bottom. \$\endgroup\$ Jul 7 at 23:13
  • \$\begingroup\$ Hmm... wouldn't it cause problems with the current sense if all 5 drivers' VOUTs were tied together? \$\endgroup\$
    – Reid
    Jul 8 at 0:31

3 Answers 3

14
\$\begingroup\$

IC Datasheet:

  • "EP Exposed pad/TAB connects to GND and thermal mass for enhanced thermal impedance."

    It doesn't say that omitting this will certainly damage the device, but in general, EP's are always to be connected to something. If nothing else, omitting it could cause the device to overheat quickly.

  • "Absolute max VSW, VSET SW, SET Pin Voltage is -0.3 to +65 V"

    For lower input voltages, this wouldn't be much of a concern. But when operating at 48 V input, just 8 more Volts is max recommended, and 17 more Volts more can destroy the device. Or in other words, this isn't a lot of "headroom."

    Anywhere an inductor is switched, is the possibility of (potentially huge) voltage spikes. It doesn't matter if the "controller should have been off" - it could have a start-up mode where it pulses once to check for operational validity and that single pulse was enough to exceed the max rating. Hence why an oscilloscope is mandatory when designing and troubleshooting a switching supply.

Now the device says it will work from 5 V upwards. In addition to all of the comments, to troubleshoot this particular incarnation of the board, I would do this:

  • Disconnect and ignore the microcontroller for now.
  • Replace one AL8862QSP-13 and desolder the rest. Check for any other failures such as open resistors or shorted capacitors.
  • Supply +6V to the regulators. With no load, they should draw very little current (0.45mA per chip at idle.) If you see something ridiculous like 50mA, stop here and figure out why. Could be that something is oscillating that shouldn't be ('scope is again your friend.)
  • Take two indicator LEDs, breadboard them in series with a 22R resistor, and connect this to a regulator output. Keep your 'scope handy to investigate what nodes are doing what. Monitor current input and device temperatures. Increase/decrease voltage slowly, methodically, while adding/removing LEDs and looking at voltages on the 'scope. If anything approaches the device maximums (even tiny spikes >55V) stop before another chip is damaged.

This particular datasheet is not the most user-friendly. It shows pin names and functions, but barely a real circuit, let alone no PCB layout recommendation or guidelines. An expert could use this well enough, but only because they've already blown up enough boards to know all of these gotchas.

\$\endgroup\$
5
  • 12
    \$\begingroup\$ "but only because they've already blown up enough boards to know all of these gotchas" you spawned some rueful chuckling there. \$\endgroup\$
    – TimWescott
    Jul 7 at 19:14
  • \$\begingroup\$ Thank you for the thorough answer! I've already updated the design to connect EP to GND. I (apparently naively) assumed the flyback diode would protect the IC from any voltage spikes from the inductor, but I gather that it might not "react" fast enough to protect the IC. I really appreciate you laying out the troubleshooting procedure as well. I'm starting to do some research into quality entry-level scopes and bench power supplies so I can walk through it. I may also revisit Digikey to see if there's an alternative driver that suits my needs, but I don't recall having many options. \$\endgroup\$
    – Reid
    Jul 7 at 20:21
  • 1
    \$\begingroup\$ If you're on a tight budget, also consider used test gear. Some good deals can be found on the big auction site. Just research items well before buying. \$\endgroup\$
    – rdtsc
    Jul 7 at 20:54
  • 1
    \$\begingroup\$ Some learn by hands-on trial-and-error. Nothing wrong with that (except maybe a slight increase in air pollution.) Not everyone is as perfect. \$\endgroup\$
    – rdtsc
    Jul 7 at 20:59
  • \$\begingroup\$ I'm always a big fan of buying older, well-built gear. Any tips on what to look for (e.g. good manufacturers)? \$\endgroup\$
    – Reid
    Jul 7 at 21:32
11
\$\begingroup\$

In addition to the answer from @rdtsc, your trace leads are far too narrow, and that, in turn, leads me to suspect your PCB layout.

You don't say what current you're running. You should analyze the circuit and figure out the RMS* current in each trace. Then you should find a trace width calculator and make the traces that long. Then you should look at the schematic, and identify each loop in the circuit where there's lots of switching current, and you should make those loops small, both to reduce stray inductance and to reduce emissions.

While you're at it, check the current through D3 -- if L3 is sized correctly, then D3 is probably too wimpy. If D3 isn't too wimpy, then L3 is probably bigger than you need.

You may want to dig through the Diodes, Inc website to see if they have an app note on this chip -- typically manufacturers make sure that there's a recommended layout available.

If there isn't such documentation, and if it makes sense within your project, I'd even go as far as to suggest that you choose a different chip that includes a recommended layout and parts list, and just copy that.

* If you've only been working on radio or AC power, or even if your engineering culture is slightly different than mine, our definitions of "RMS current" may be different. Note that when I say "RMS current" here I mean you should find the mean of the square of all of the current, both DC and AC components -- some people may call it the "DC + RMS" current.

\$\endgroup\$
5
  • \$\begingroup\$ Thanks! The drivers are supplying 1A, which (from a thermal standpoint) is easily handled by my trace widths according to IPC-2152. Maybe I'm just dumb (remember, I'm a mechanical engineer), but wouldn't the RMS current just be the set point of the drivers? I really tried to make the LED +/- leads as short as possible, but it was a real struggle to get it even as good as it is in this design without having a million vias. Maybe smaller inductors would let me squeeze everything tighter. \$\endgroup\$
    – Reid
    Jul 7 at 20:27
  • \$\begingroup\$ You want fat traces to bring the inductance down, too. \$\endgroup\$
    – TimWescott
    Jul 7 at 23:51
  • \$\begingroup\$ Any thoughts on how fat is fat enough? It's looking like 2mm is about the limit, and even so I'm having to do 1mm for the traces connected directly to the driver's pads. \$\endgroup\$
    – Reid
    Jul 8 at 1:57
  • 1
    \$\begingroup\$ As fat as you can make fit. Coming off of the driver with a thin trace then fattening it up is a done thing, too. \$\endgroup\$
    – TimWescott
    Jul 8 at 22:46
  • \$\begingroup\$ Suggest looking at other switching regulator datasheets which do have layout examples. Study those carefully, and apply that methodology to your design. \$\endgroup\$
    – rdtsc
    Jul 16 at 14:03
2
\$\begingroup\$

To add to @Reid's and @rdtsc's observations, I noticed that the data sheet for the AL8862Q indicated that the FAULT pin ought to be connected to VIN via a pull-up resistor. I'm not familiar with this chip, but I wonder if the lack of the resistor might have an unpleasant side effect like oscillation that cascades into the failure mode you encountered.

\$\endgroup\$
2
  • 1
    \$\begingroup\$ Thanks - since the datasheet shows FAULT floating in their typical circuit, I took that comment to mean a pull-up resistor was needed only if you wanted to be able to monitor fault condition (by the pin being pulled low). \$\endgroup\$
    – Reid
    Jul 7 at 21:39
  • \$\begingroup\$ Again, it is better to have the option, but you do not need to populate it. \$\endgroup\$ Jul 8 at 1:46

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.