0
\$\begingroup\$

I have PCB printed a board that feeds a 12V led strip from either a Li-ion battery or a 5V USB. With no load, the output is 12V, as it should. As soon as I connect the led strip (80mA at 12V), the output voltage drops to ~8V, and the current drops to a few mA. The circuit also produces a distinct high-freq sound when a load is connected. However, the circuit works fine with other input voltages. Below is the list of working and non-working input voltages, and the current:

  • Vin < 3.0: does not work (expected)
  • 3.0 < Vin < 3.7: works, I ~ 450 mA
  • 3.7 < Vin < 5.5: does not work, I ~ 20 mA
  • Vin > 5.5: works, I ~ 240 mA

The current flows from the top to the bottom in the pic below. It's a one-sided board.

C4: 25V 22uF X5R ±20% 0805

L1: 2.3A 10uH ±20% SMD,5x5mm

D5: 40V 0.45V 5A DO-214AA Schottky

Version 1

enter image description here enter image description here

Questions:

  1. why does it behave like this?
  2. how can I fix it?
  3. can I fix it without re-printing the PCB?

There are related questions:

but the former hasn't shown how far the capacitor had been placed in the beginning (is my cap C4 placed too far or acceptable?) and after he found the solution, and the latter seems to be not resolved, only hints.


Version 2

After reading the replies, I updated the layout as follows:

enter image description here


Version 3

Where possible, replaced tracks with copper pour.

enter image description here


Version 4

Tight SOT23-6 footprint, removed R_EN.

enter image description here


Full project link: https://github.com/dizcza/flashlight_kicad

\$\endgroup\$
10
  • \$\begingroup\$ In your list of input voltages/currents, is the current value the input current at that voltage for the same 12V 80mA load connected on the output? Also, are you able to probe the output voltage? \$\endgroup\$
    – LordTeddy
    Jan 10 at 22:53
  • \$\begingroup\$ There is a very long way from C3 GND to U2 GND and even longer to R6 GND. Can you improve this somehow? \$\endgroup\$
    – Jens
    Jan 11 at 2:37
  • \$\begingroup\$ @LordTeddy yes, the list shows V and I for the same load (12V 80mA connected directly to my adjustable power supply). I can probe the output voltage and that's how I noticed the voltage drop. \$\endgroup\$
    – dizcza
    Jan 11 at 7:36
  • \$\begingroup\$ @Jens yeah, I think I need to do another schematic just to test it. But should also I add 100nF caps to both input and output not to mention that they should be closer to the U2 now? Should I add a bulky 680uF to the output as in the second schematic I linked as related? The value of the L1 inductor does not play a role here and I can still use the same, 10 uH? \$\endgroup\$
    – dizcza
    Jan 11 at 7:43
  • \$\begingroup\$ @Jens Thanks for pointing this out: placing them physically close does not mean that the path to GND is short, I'll pay attention to this. Is this the only crucial mistake I made here? \$\endgroup\$
    – dizcza
    Jan 11 at 7:48

2 Answers 2

2
\$\begingroup\$

There is a very long way from C3 GND to U2 GND (red) and even longer, leaving the picture, to R6 GND (orange). This should be made drastically shorter.

GND paths in the layout

If the SW output is on, the current flows along the red path, if the diode is conducting the current flows along the yellow path.

These long tracks behave like additional inductors L2, L3 and L4. The MT3608 will read wrong values at the FB pin because the GND pin voltage is different from the GND potential of the capacitors. So the IC makes wrong decisions. The track inductance L2 adds voltage ringing at the IN pin, L4 at the output circuit.

The generated EMI from these large loops also is a mess.

enter image description here

\$\endgroup\$
11
  • \$\begingroup\$ Thanks for the equivalent schematics - that's very educational. Shortening the GND paths manually, I noticed that in my case it's sufficient to shorten the R6 GND only, and shortening C3 GND to U2 GND is optional. I did both, however. "The MT3608 will read wrong values at the FB pin because the GND pin voltage is different from the GND potential of the capacitors" - I thought the C3 and C4 are just bypass capacitors, aren't they? \$\endgroup\$
    – dizcza
    Jan 21 at 8:05
  • 2
    \$\begingroup\$ @dizcza The only "traces" should be to feedback components. The switching power path - anything connected to C3, L1, D5, C4, and U2 pin 1,5,2 should be copper pours, laid out for minimum distances between paths. There should be plenty of vias from top-layer GND pours to a ground plane on some other layer. the C3 and C4 are just bypass capacitors, aren't they? No. They are the capacitors through which the switching currents flow. Without them, the regulator will likely self-destruct for example. Their parasitics have direct impact on performance, and they are critical parts. \$\endgroup\$ Jan 21 at 22:39
  • \$\begingroup\$ @Jens could you have a look if the updated layout doesn't have other issues that I missed? I'll be placing a new order soon and want to make sure this time it will work. Thanks. \$\endgroup\$
    – dizcza
    Jan 23 at 20:48
  • \$\begingroup\$ Looks much better now. Do you use X7R capacitors? \$\endgroup\$
    – Jens
    Jan 23 at 22:19
  • \$\begingroup\$ @Jens no, they are rated X5R. I see that X7R are recommended but I really don't know if selecting X7R is crucial here. I'm trying to minimize the assembly price and for X7R caps I need to pay extra $3.00 because it's from "Extended Lib" of JLCPCB while X5R 22uF can be found in basic components with no extra cost. I've linked my full project with BOM. \$\endgroup\$
    – dizcza
    Jan 24 at 8:29
2
\$\begingroup\$

When making high-frequency switchers, one should always follow "reference designs" and recommended board layouts, due to presence of "high-current loops" in switching converters. Can you see the differences between your layout and the reference? I would also try to follow the reference BOM, because some overlooked parasitics of components may affect declared performance of the device.

enter image description here

\$\endgroup\$
2
  • 1
    \$\begingroup\$ For things like sensors and uC, I look at hardware integration files. And I did look at MT3608 datasheet but I didn't pay attention to the recommended layout (I thought why should I care about the layout for such simple things as step up/down regulators). How wrong could I be... I'm marking @Jens' response as the answer as he pointed out the issue first in the comments. \$\endgroup\$
    – dizcza
    Jan 21 at 7:54
  • 1
    \$\begingroup\$ @dizcza Modern high frequency switching regulator performance is largely determined by the layout, especially the EMI performance. why should I care about the layout for such simple things They are far from simple, textbook simplifications notwithstanding. In a switcher, the layout is basically everything, and with the exactly same components the layout will determine whether the thing works well, poorly, not at all, or even self-destructs. Yup. The layout you have made is pretty much exactly what not to do :) Essentially every thing you could get wrong, you did get wrong :) \$\endgroup\$ Jan 21 at 22:36

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.