LM5118 power supply board Problems.

[bbqstingray]

Hello all,

I am trying to design a power board with 24V/12V/6V rails with the LM5118 buck-boost chip. The voltage regulation of the buck-boost is 24V which will then supply the 12V rails and the 6V rails.
However,  when testing the boards I encountered some problems.

Problem 1:
When i supply my board with 22.4V battery pack, the 24V Voltage output only outputs ~ 5-8V which will only power up the 6V rail (L7806CV-DG) but not my 12V rail (OKI-78SR-12/1.0-W36-C) even when there is no load attached to it.
Similarly, when testing with a DC power supply, if I supply a voltage of above 10.2V the same voltage output occurs. If a low output voltage occurs when connected to the DC power supply, I can lower the voltage to below the specified UVLO pin shut off (currently set to ~9.8V but will change for the next board revision) and it the buck-boost vout is 24V and the other voltage rails are supplied. I am not 100% sure why this occurs. I have attached the schematic and my PCB layout in the zip file below. The PCB design has a top layer 

Problem 2:
After the DC power supply 'hot fix', another problem I am encountering Q1 MOSFET is heats up when the current very quickly when a 6v pump is attached. Looking at Vgs of the looks to be about 2V which can lead to a high heat for the MOSFET but is there a way that I can change the voltage drop of the Vgs so that it will have less power loss?



Please note that I have replaced Q1 MOSFET to RSJ301N10FRATL - https://au.mouser.com/datasheet/2/348/rsj301n10fratl-e-1873400.pdf
6V rail - L7806CV-DG - https://docs.rs-online.com/2f50/0900766b8163480b.pdf
12V rail - OKI-78SR-12/1.0-W36-C - https://au.mouser.com/datasheet/2/389/cd00000444-1795274.pdf
buck-boost model - lm5118MHX -  https://www.ti.com/lit/ds/symlink/lm5118.pdf?ts=1628175667672&ref_url=https%253A%252F%252Fwww.ti.com%252Fproduct%252FLM5118

[prasimix]

I experimented with the LM5118 few years ago. At first I can say that the PCB looks anything but optimal, I'm not sure that the layout of the power loops was taken into account, the widths of the traces are insufficient, and low ESR (ceramic) capacitors are missing both at the input and output. Putting only elco's is not enough even those called low ESR.

[JonasCz]

LM5118 (and any switching regulator for that matter...) is very sensitive to layout - it will indeed behave erratically if the layout is not done very carefully. The datasheet has a short section on layout showing the critically important bits, namely the current loops and and (ground) planes needed.

I'd generally use 4 layer board for something like this, it makes layout much easier and usually gets better performance.

Your schematic looks OK with a quick look, I don't see anything obviously wrong. Add some ceramic caps (~few uF maybe?) on the input and output though.

[bbqstingray]

Hi Prasimix and JonasCz

Thank you for taking the time to give me some feedback. 
Sorry it’s taken a bit of time to reply. 
I have re-layout my board and increased the number of layers of my board. 
•   I have increased the number of bypass caps at the input and output of the regulator
•   Layers so far are L1-Signal, L2-GND, L3-Power (24V regulated output), L4-Signal. 
•   I have increased the number of vias around the 24V bypass capacitors and GND. According to this Phil’s Lab youtube channel (link, at time when he says adding vias would reduce inductance.
        https://youtu.be/C7-8nUU6e3E?t=8338)

Could you please review my revised board layout.
And thank you for giving me feedback, it was much appreciated.

Cheers

[mariush]

How much current do you need on each rail?

I see the switching regulator you chose for 12v outputs maximum 1A of current, and needs 15v ... 36v input voltage.  You may do better using a SEPIC regulator chip that can do 10-24v to 12v instead of boosting to 24v only to buck down to 12v (you're losing energy in conversions)


You chose a linear regulator for the 6v output. A few bad things about it :
* it's kinda of a bad idea to use a fixed voltage 6v version of a chip, because you may run into availability problems (no stock) in the particular format you want (ex to-220)
* it's a linear regulator, so the difference between input voltage and output voltage will be dissipated as heat ( ex 24v in , 6v out at 50mA  = (24-6) x 0.05A = 0.9 watts of heat.
* you chose the to-220 version, which means it sits above the pcb susceptible to vibrations and all that, and you may need to add a heatsink to keep the chip cool.

I would suggest changing the part to something adjustable, like let's say a LM317 or LM1084 or maybe even a 1117 regulator (but I avoid these 1117 regulators as SOME models are sensitive about ESR on the output, requiring an electrolytic capacitor with esr between 0.1 .. 1 ohm, or adding a resistor in series with the ceramic capacitor on the output to increase the ESR)
Two extra surface mount resistors could save you a bunch of time trying to find a fixed 6v regulator.

Note though that some of these regulators may not be capable of 24v input voltage, but I wouldn't recommend powering them from 24v in the first place.

If it HAS to be a linear regulator rail, I'd suggest powering this 6v rail from the 12v rail, and basically have this 6v rail also act as a minimum load for the 12v rail. 
You may have to use a better 12v switching regulator, capable of more current

Also, depending on how much current your 6v rail uses and the heat dissipation, I'd suggest using a DPAK / to-252 package (surface mount the regulator) and have larger copper pad and some vias go to the bottom of the board and now you don't need separate heatsink for the 6v regulator


You may also want to investigate if it's not just easier to use a boost only regulator for the 24v output if you're sure your input voltage will never be higher than 24v and use a SEPIC regulator just for the 12v rail.

Could just specify 7.5v...20v input voltage (or 12v..20v) and be happy with that. Would allow powering from ATX power supplies, would also allow powering from laptop adapters with 16v..20v input, also usb type c power delivery does 20v...

I see you use 1206 ceramics in lots of places ... no need for that on decoupling capacitors.  Use 0805 or even 0603 (if your eyes can handle it) ... and for 100nF ceramics, you can do X5R also, if they're available in higher quantity or cheaper price at certain quantities.
You have some 1nF and 22nF in 0603 package so it doesn't look like you're scared of the size.

Think of simplifying your bom -  i see a 33k resistor, I see a 15k resistor , I see a 20k resistor , i see two 18.7k resistor  ... if you're stuck with 18.7k in two places, maybe you can change the 20k to 18.7k and do the math to adjust the 33k resistor (i see a note about shutoff point at 33k-20k divider so maybe not doable but think about it)
Could you maybe change the 15k resistor in the compensation to another 18.7k and adjust the capacitor value? Do the math
Also a 1meg and a 510k resistor ... maybe use two 1 meg in parallel to get 500k and that should be close enough.


I see a 68uF 100v alu smd ... is that electrolytic surface mount?  Those are kinda known to leak eventually? Does it have to be 100v rated? You can probably find lower esr polymer capacitors rated for 35v which should be enough ... see : https://www.digikey.com/short/qtb218m8