Problems with Power Supply using LT8609EMSE#PBF

[Rikr09]

Hello!

I'm working with the LT8609EMSE#PBF to supply voltage to Raspberry Pi Zero W mini PC and i'm getting many troubles with this regulator.

If the Vin voltage is 12V the Raspberry works without problems, turns on it Wi-Fi module and never reset itself.

Now, if the Vin voltage increase more than 12.3V the Raspberry begins to restart and never turns on it Wi-Fi module.

This also happens with a Orange Pi H2 module. So i don't know what to do.

I changed the R2 resistor value to 182k because if i put the recommended 18.2k the voltage drops to 3.9V or less once the Raspberry begins to configure itself and consequently it wont work either.




I hope you can help me with this.

Best regards,

 

[barry]

My guess is either you don't have this wired correctly, or you've got a bad PCB layout. The fact that running it a lower frequency (larger Rt) makes it work better definitely points to a layout issue.

What is your load current?

 

[KlausST]

Hi,

* unsuitable inductance
* unsuitable PCB layout
* unsuitable capacitors

Give us the according informations, so we can verify it.

Klaus

 

[Rikr09]

My guess is either you don't have this wired correctly, or you've got a bad PCB layout. The fact that running it a lower frequency (larger Rt) makes it work better definitely points to a layout issue.

What is your load current?

Hello, thanks for your reply,

Is 100mA maximum.

- - - Updated - - -

Hi,

* unsuitable inductance
* unsuitable PCB layout
* unsuitable capacitors

Give us the according informations, so we can verify it.

Klaus

Hello, thanks for your reply.

Below are the schematics and the corresponding PCB Layout, also the typical application recommended by the manufacturer in the datasheet.





I hope you can help me with this.

Best regards,

 

[barry]

This is not really clear. Is this a bottom view? Are you showing topside traces looking from the bottom? Why??

Is this a two layer board? Then the bottom layer under the circuit should be solid ground plane.

The input capacitor, C2, could be closer to the IC. Again, read the section on PCB layout in the data sheet. You might try putting a small cap from pin 10 to ground and see if that helps.

Here's another thought. Maybe try adding a resistor on the output to maintain a minimum load of a couple of milliamps.

 

[FvM]

This is not really clear. Is this a bottom view? Are you showing topside traces looking from the bottom? Why??

Is this a two layer board? Then the bottom layer under the circuit should be solid ground plane.

Everything becomes clear at second sight. It's a two layer board, all SMD components are mounted on the bottom side.

The really bad thing is the dissected ground, e.g. C2 and C6 not directly connected to U1 ground pad, the return path is not even visible inside the screenshot. U2.9 to C2 to U1.11 is the commutation loop where the switcher input current is circulated. Apparently it's routed allover the board. This could be improved a lot by placing a few additional ground vias. Better rotate C2 by 180° and connect to the upper ground pour. This can be a fix to the existing PCB.

 

[KlausST]

Hi,

As already written: It´s very likely that the PCB layout causes problems.

But I mentioned two other possible problems:
* inductor
* capacitors

Show us (a link to) the datsheets.
Both need to be well chosen - thus there should be an extra section in the datasheet.

Klaus

 

[Rikr09]

This is not really clear. Is this a bottom view? Are you showing topside traces looking from the bottom? Why??

Is this a two layer board? Then the bottom layer under the circuit should be solid ground plane.

The input capacitor, C2, could be closer to the IC. Again, read the section on PCB layout in the data sheet. You might try putting a small cap from pin 10 to ground and see if that helps.

Here's another thought. Maybe try adding a resistor on the output to maintain a minimum load of a couple of milliamps.

Hello!!

You were right, according with the PCB layout suggestions, the C2 must be closer to the IC and i did that and inmediately begins to work as expected. Thanks for that! :-D:-D:-D:clap::clap::clap:

PD: The only thing that i don't know why is not working is that i increase the input voltage to 36V and the IC burnt.

 

[barry]

The internal LDO regulator may be overheating.

 

[Rikr09]

The internal LDO regulator may be overheating.

And... how i could fix this? According with the datasheet this IC should stand until 42V.

 

[KlausST]

Hi,

According with the datasheet this IC should stand until 42V.

That´s the key point. 42V is not the average voltage, it is the max. peak voltage. Any peak that crosses this 42V border may cause damage.

--> With inappropriate layout you get much higher voltage peaks than 42V.

Klaus