0
\$\begingroup\$

I am creating two part PCB running on Li-ion battery 26650 (3C discharge rating, max capacity 5000mAh) powering few LED strips with controller. PCB 1 (schema 1) has step-up converter MT3608 which steps up battery output to 5V. LED strips requires 5V. Battery is placed on 2nd PCB with battery controller circuit (schema 2).

Issue: PCB 1 more likely MT3608 not provide enough amps to run LED strips (0.7A max in basic mode) & controller (ESP32 ~200mA) however MT3608 should be able to deliver 2A (I need 1.5A top). If I power up PCB 1 directly via ESP32 usb connector then Windows run audio about disconnecting USB but both devices are running well (also tried powerbank 2A delivery, works, input ESP32).

I think there is issue with MT3608. I disconnected PCB 2 and used computer PSU with 3.3V node. Still not working. When devices freeze I can hear loud noise coming from power inductor. Running just ESP32 without LED part is just fine for ESP32. Plugging in LED connector makes ESP32 crash.

Schema PCB 1 enter image description here VIN => 3.3V (PSU) | 3.7-4.2V (Li-ion 26650)

Some parts are not soldered onboard

Schema PCB 2 enter image description here I can post up PCB wiring if you need.

I did some measurements. TYPE | 5V node | VIN ESP32

26650 | 4.6-4.7 | 4.7

PB | 4.3-4.4 | 4.3

PSU | 2.8-2.9 | 2.9

PB => Powerbank PSU had 3.3V There is for sure some voltage drop on PCB 1.

Any idea what to improve?

Layout PCB 1 - MT3608 part enter image description here (line on the right goes to VIN ESP32)

Datasheets:

Power inductor

Diode

22uF caps

\$\endgroup\$
  • 1
    \$\begingroup\$ Your schematic is a mess. Schematic should flow from top to bottom, left to right. Also, D2 will prevent your circuit from working. \$\endgroup\$ – Lior Bilia Apr 24 at 12:26
  • 1
    \$\begingroup\$ I suspect inductor saturation, so you'll have to post the inductor datasheet. Also it would help to see the layout and more info on input/output caps and diode. \$\endgroup\$ – bobflux Apr 24 at 12:55
  • 1
    \$\begingroup\$ Got an oscilloscope? \$\endgroup\$ – bobflux Apr 24 at 12:55
  • 1
    \$\begingroup\$ Lior is right about the schematic. Tips: (1) Turn the battery right way up. + on top. (2) Use ground symbols for everything connected to battery negative and remove all the negative wires. Always have the ground symbols point downwards towards, um, the ground. (3) If Q1 is a pair of MOSFETs (DGS, I'm guessing) then use MOSFET symbols. You're trying to show the *schema", not a wiring diagram. (4) Move VIN to the left if it's an input. General signal flow would usually be from left to right. Current flow would be from top to bottom. (5) Eliminate unnecessary kinks such as the one from OD to G1. \$\endgroup\$ – Transistor Apr 24 at 12:55
  • 1
    \$\begingroup\$ (6) Turn off the grid for screen grabs. (7) Have fun! \$\endgroup\$ – Transistor Apr 24 at 12:55
2
\$\begingroup\$

Inductor datasheet does not spec saturation current, but it does spec max DC current:

enter image description here

With 0.11 ohms DC resistance, at 1.23A it will dissipate 0.16 Watts. An inductor of this size (7.3mm x 7.3mm) can dissipate a lot more heat than this without overheating, therefore I believe the max DC current is not specified with regards to maximum temperature but with regards to magnetic saturation.

So we have a saturation current value, and unfortunately it is too low if you need 1.5A on the 5V output. You should calculate peak inductor current and select an inductor with a saturation current specification a bit above this. Note peak inductor current is higher than average input current, you must calculate it. Here's a guide.

Now the layout...

enter image description here

The chip switches inductor current between the cyan and blue paths which are the "hot loop" and that should have a very tight and short layout. If possible blue and cyan paths should be as close as possible to each other.

Also the inductor current path (green) and the path between GND of input caps, output caps and the chip should be as tight as possible.

This layout is pretty bad, I think the ground pour made you think "GND" was connected everywhere but look at the path the current has to take through the ground pour... this will radiate a lot of EMI and it probably won't work at all, considering the high switching frequency.

enter image description here

For this kind of layout, you should place the chip, input caps and output caps in such a way that the GND pins of the three components are connected together very close and tight. Then place the diode and inductor.

Highest priority is the hot loop, then inductor and input cap, then the resistors, which are low priority.

If you have a ground plane on the other side it's easier because you can use vias, but if you don't, then you have to make a real good single side layout. At this switching frequency a ground plane is pretty much required...

You can look at layout advice in datasheets of other boost converters in SOT23 packages. Manufacturers like TI or AD usually provide good hints.

Edit: quick'n dirty layout fix

Pushing high di/dt current (in this case a >1MHz current square wave) into an inductive path (long winding path) radiates lots of EMI but it will also cause voltage spikes to appear between various points labeled "GND" along the way. This can make your DC-DC chip misbehave, for example if the spikes find their way in the feedback the chip might think the output voltage is wrong and do stuff you don't expect (like shutting down).

You can scratch the soldermask, drill some holes and solder wires through the board to the ground plane on the other side to create vias (green dots on the picture) on the important GND pins. This will make a much shorter and less inductive ground connection.

enter image description here

This should fix some but not all EMI problems, and I think it'll probably work if you use a suitable inductor.

If you redo the board you can post a "check my layout" question and ask for advice.

| improve this answer | |
\$\endgroup\$
  • \$\begingroup\$ Thanks for explanation. I tried my best with layout, doing it first time, tried to make it short as possible. Bottom layer is covered with ground aswell.. Thanks for advise. Can I fix current PCB with better inductor to get this working or I have to redesign layout? \$\endgroup\$ – oflfo Apr 24 at 14:42
  • \$\begingroup\$ Don't blame yourself, it's a very common mistake... And you can make vias with a drill and probably make it work, I've added some explanations. Good luck! \$\endgroup\$ – bobflux Apr 24 at 15:21
  • \$\begingroup\$ Ok I will first try to replace inductor. I guess its not last iteration for this idea :) \$\endgroup\$ – oflfo Apr 24 at 16:34

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.