* Please post a link to a public copy of your project.  * Please post a description of how this circuit works including a description of what each device is, a link to it's manufacturer's datasheet and what it's function in the circuit is.  * Also provide a more detailed description of what appears to be the problem and under what conditions it appears. "...but it seems not stable. Can anyone suggest what did I do wrong in my design? and how to improve it. I'm suspecting the latch parts has the issue as I ground it from Bat-. " is less than helpful when it is not obvious what the circuit is intended to do and what the individual device are that it is made up from and how it is laid out on the PCB. <br> Thanks.

Hi! I think there is a few things to improve: 1) C1 should be 100nF 2) R1 is quite high value for a LED current limiting resistor 3) There should be 10uF ceramic capacitor near pin 5 of U1 4) C2 and C4 are incorrect, they should be 22uF ceramic/tantalum capacitors. Keep the 22nF caps though in series with the 22uFs, helps with the high frequency ripple 5) R8 and R9 are quite high value. Drop down half of the resistance, say somewhere to 47k 6) R10 is quite high, drop a decade. (10k) Alright, thats the initial list to go through, then we get to the latch. I assume you press the latch to test? When you release the latch the MOSFET stops conducting? Same thing with the transistor Q2. You set high to the gate and Q2 conducts and therefore MOSFET starts conducting. You set low and Q2 stops conducting and MOSFET stops conducting. Then there is a pad with SIG, do you feed a signal there or just use it to measure the voltage? Same with TRG, I assume it is a switch. Other than that, the rest is just a guesswork. Just as Andy said there, the additional information is required to make more sense of this module. The PCB layout is an additional set of things that can affect to the functionality of the circuit if it is not layed out properly. Regards, Markus Virtanen HW / Electronics Designer

@markus_jidoka, @najibabdullah, In your point (4) you said: "Keep the 22nF caps though **in series** with the 22uFs, helps with the high frequency ripple" Did you mean "... **in parallel**..."? :)

Hi Andy! Yes! In parallel Sry! My mistake :-( -Markus

@markus_jidoka @andyfierman Hi Markus and Andy, Thanks for your reply and suggestion. Kindly refer to this link for the project [https://oshwlab.com/najibbinabdullah5609/li-ion-charging-boost-protection-3-7-5v](https://oshwlab.com/najibbinabdullah5609/li-ion-charging-boost-protection-3-7-5v)<br> <br> The issue is: 1\. Output voltage is not 5v even though I use the ratio of R1=7\.5K and R2=1K\. The Vout Theoretically will output 5\.1V\. 2\. When I scope the voltage across the VOUT\+ and VOUT\- I'll get the below signal without push the latch button\.  The idea of having the latch switch there is when I press the button it will turn on my MCU, where TRIG pin will set high during the press period. When the latch button release, TRIG signal still hold the transistor Q2. The SIG pad connected to MCU to read the status of the button. So I can turn off the circuit programmatically by set TRIG pad low from MCU. I want to control GATE Q5 to cut off the voltage. I have the board soldered and the results is not as expected\. There's a suggestion to relocate the latch switch before the booster part\. Did I correctly connect the GATE of Q5 to BAT\- or should it connect to BAT\_TER\-\. From the schematic\, the BAT\_TER\- and BAT\- is not directly connected\. <br> <br>

hi @markus_jidoka, Do you mean need to add another 2 [Tantalum Capacitor](https://www.electronics-notes.com/articles/electronic_components/capacitors/tantalum.php "Tantalum Capacitor » Electronics Notes")  in parallel to the C2 an C4? <span class="highlight"></span><br> <br>

@najibbinabdullah5609, Tantalum or aluminium electrolytics should workbook but you should check the datasheet recommendations on the MT3608 datasheet. Without seeing the design calculations for the MT3608 boost converter it is unclear what ripple current rating is required for C2 (and to a lesser extent, C4).

Autocorrupt: workbook = work ok

Hi @najibbinabdullah5609 Yes, the most likely problem is that your boost converter doesn't produce steady 5V because there is no tantalum / ceramic capacitors in the input and the output. If there is not if enough capacitance especially in the output, then the boost converter can't regulate the output and therefore oscillates. I recommend to use something like these from LCSC: **THT:** _C454407_ or _C62893_ **SMD:** _C140602_ or _C782264_ Regards, Markus Virtanen HW / Electronics Designer

Usually default value input and output capacitors work mentioned in the datasheet. However, this is a case by case situation. Sometimes you need to "tweek" your capacitance in order to achieve a better boosted voltage regulation. -Markus

@markus_jidoka Thanks bro.. Any comments or feedback on the latch switch part?

Hi @najibbinabdullah5609 As soon as you make the component changes around the latch switch part then I do think it works. But in order for me to be 100% sure, then I should build it myself and test it. I just took a look at your PCB file and as a professional layout engineer I see many rookie mistakes. Heres a small list to improve it: 1\. Try to keep one signal trace on a single layer and jump as few layers as possible\. Your BAT\_TER\+ power signal jumps between layer eight times\! 2\. The center part of your PCB is like a jungle\, signals flying everywhere :\-\(  3\. The booster regulator is not layed out properly\. IC\, coil\, diode\, capacitors and voltage setting resistors should be a tightly spaced together and not like this where these components are located separately all the way to the other sides of the PCB 4\. Silkscreen is not optimally spaced\, some letters are partially missing 5\. Copper area properties are default values\, I suggest to tweak them a bit\. a) Clearance: 0.016" b) Pad. spokes c) Spoke width: 0.024" d) No islands! e) Solid fill f) Copper to outline: 0.016" g) Yes h) No 6.You only have one via on Vout+, I suggest add a couple more 7\. Trace widths are not ideal\. Power and signal trace widths differs alot 8\. Placing vias on component pads is usually not recommended if you use JLCPCBs SMT service but ok if you solder the components by yourself OK, that a small list that can greatly improve the functionality of your PCB. Let me know if you need a professional layout service from me, I am up for a hire :-) Regards, Markus Virtanen HW / Electronics Designer

Hi @markus_jidoka , Thanks for your comments and suggestions. That's a great idea.. Can we discuss in detail your service? You can reach me at my email [najibbinabdullah@techcareinnovation.com](mailto:najibbinabdullah@techcareinnovation.com).

Hi! I sent you a email, hopefully you got it?

You'll need to study the datasheet for the MT3608: [https://www.olimex.com/Products/Breadboarding/BB-PWR-3608/resources/MT3608.pdf](https://www.olimex.com/Products/Breadboarding/BB-PWR-3608/resources/MT3608.pdf)<br> <br> It is not very good but at least gives a recommendation for X5R or X7R dielectric **ceramic** 22uF input and output caps. Since this device switches at about 1MHz, tantalum and aluminium electrolytic caps are **not** suitable, as I incorrectly suggested earlier. The datasheet recommends referring to the inductor saturation current rating without giving any information about how to scale this value with inductance value, load current and (output-input) voltage difference. Using the switch current limit of 4A as a guide, since this is the peak current that the inductor must handle during an output short circuit event, is OK but that may result in an over specified inductor current rating for an embedded application where a short circuit results from the failure of some other component so the switcher failing is a secondary fault. Although having the switcher catch fire may be a less than desirable outcome of a shorted output rail... * If you want to calculate the inductor (and diode) value and ratings correctly using verified formulae that are not given in the MT3608 (and often only given in simplified form in many datasheets and other sources) then please see this project and run it in Sim mode: [https://easyeda\.com/andyfierman/Simple\_Open\_Loop\_Boost\_Converter\-iuoiASasK](https://easyeda.com/andyfierman/Simple_Open_Loop_Boost_Converter-iuoiASasK)<br> <br> Editing the **Design Requirements** section of the spice statements on the right of the simulation sheet will allow the sim to run in the conditions that your application is expected to. By adding an input capacitance and editing the value of the output capacitance, this sim can also be used to specify the voltage and ripple current ratings for these two capacitors. The second sheet shows the design calculations that are used in - and verified by - the simulation.

Sorry, missing information: "By adding an input capacitance and a small source resistance in series with the input voltage source..."

Hi! @najibbinabdullah5609 It seems that your organization blocks my emails to you. I have tried with my gmail and hotmail accounts and both gets blocked and bounced back :-( The error says: "Message bounced due to organizational settings."

@najibbinabdullah5609 Can you private message me and give a personal email account name?

@andyfierman Thanks Andy, I'll look into this. To be honest I just try out design all this following other people circuit without really understand why we should choose the component value. I still need to learn about electronic. Thanks for your help. Thanks and regards, Najib Abdullah

@najibbinabdullah5609, "To be honest I just try out design all this following other people circuit without really understand why we should choose the component value." Particularly if you are working with switched mode supplies and lithium ion batteries that is a very risky "design" strategy. Electronics is not like Lego. Having a switch mode supply or a lithium ion battery explode in your face as you are debugging the charger circuit is not a good design outcome. "I still need to learn about electronic." If you need design help on other projects, you are welcome to contact me through: signality.co.uk.

Hi Andy! Don't worry, Najib hired me to do the improved schematic design and PCB design for this project. He is now "in my safe hands" :-D Regards, Markus Virtanen HW / Electronics Designer

@markus_jidoka, Good to know there are people around on the forum who can help out. :)