Request for Feedback on Board Layout: 1.2Mhz Switching Boost Converter 12V-20V

[zachary5577]

I'm looking to get some feedback on this boost converter board that I've layed out.  Is there such thing as too many vias?  My guess would be that having all of these here like this would make production of the board more expensive.  Do you only put down ground vias when you need to stitch some islands and on the ground pads of your ics or in special RF cases?  Or do you ever just "go ham" with placing your vias?

I'm of the mind that, if you can't think of a good reason to do something - don't do it because it will likely just add complexity but idk.  Can you spot anything else on there that's obviously bad practice?

[zachary5577]

Just following up!  Any feedback is much appreciated!

[Martinn]

Schematic would help.
I have never seen, used or needed that many vias on any (non-radio) board.
What is the layer setup? Looks like two layers? Polygon fill seems to be missing?

[trobbins]

Definitely need a schematic, as I can't even identify an input decoupling cap (?!).

[ArdWar]

Is Q1 supposed to cut off the Vin? Why not simply use EN/SHDN pin?
Is that SMD thing between U1 and L1 supposed to be input cap? Is C2 the output cap? Looks way too small for the purpose
What is Z3 even doing? Is it supposed to be TVS or is it reverse polarity crowbar? Ditto Z2, certainly not actual zener right?

[zachary5577]

Schematic would help.
I have never seen, used or needed that many vias on any (non-radio) board.
What is the layer setup? Looks like two layers? Polygon fill seems to be missing?

Right-0!  Attached is the schematic for the board.  I've also attached a sim.

Definitely need a schematic, as I can't even identify an input decoupling cap (?!).

See attached.  Also, do you mean adding a cap on Vin?  This latest board is being updated because it was diing out in the field.  We believe there are some unexpected transients on Vin (connected directly to a lead-acid powering other things) but we weren't able to see any here in the lab.  But I've read that it would be a good idea to add an ESD cap on the input.  Probably should have added that

Is Q1 supposed to cut off the Vin? Why not simply use EN/SHDN pin?
Is that SMD thing between U1 and L1 supposed to be input cap? Is C2 the output cap? Looks way too small for the purpose
What is Z3 even doing? Is it supposed to be TVS or is it reverse polarity crowbar? Ditto Z2, certainly not actual zener right?

Thanks for asking - these are good questions.

WRT the EN/SHDN pin, the way these switching iC's work is that they have an internal fet that connects the output of the inductor to ground to build up the mag field which then opens and the voltage across the inductor + your input voltage ends up on the output.  When the IC is shutdown, it simply disables the switching of the fet - but the input voltage can still be seen on the output and draw current.  An IC that proberly disconnects VIN from VOUT would have a feature like "true shutdown".  In any case, Q1 is a highside switch to actually cut vin from vout.

Yes, between L1 and U1 C1 is the input cap.  C2 is the output cap.  Both are 0805 pkg.

Z3 really should be a TVS diode I think but no it is unfortunetly just a plain old 15V zener.  I'm hoping to swap it out for a TVS after a bit more testing.  It's supposed to clamp transients on Vin.  Here you can see of Z3 effect on a 30V pulse before and after  adding it in https://imgur.com/gallery/h54cdK3.  It clamps it down to 20V and after repeated test, this ic is still kickin (absolute maximum input voltage is supposed to be 16V for U1) but ideally it would clamp down to 15-16V.  Z2 is actually a 10V zener.  Again it's to clamp the gate voltage since it should not exceed 20V.

This is the second iterration of this board.  We were having troubles with Q2 and U1 diing previously.  After poking around, our best guess was ESD (shit answer) or a transient that we weren't able to replicate in the lab.  We increased the gate resistor of Q2 from 10ohm to 10k and added a 10V zener on it's gate.  And also added the 15V zener across Vin... Whomp Whomp.

[trobbins]

Links don't work.  Unless this is a micropower converter it will at least need a significant input bypass cap (ie. much more than 0805 smt).  Perhaps you need some more experience with smps design and benchwork ?

[zachary5577]

Links don't work.  Unless this is a micropower converter it will at least need a significant input bypass cap (ie. much more than 0805 smt).  Perhaps you need some more experience with smps design and benchwork ?

Updated the links.  Thanks.  As for experience, this is it!
WRT input bypass caps, what are we talking here? mF?  And are you suggesting putting that between Vin and Gnd?

[Martinn]

Quoting from the datasheet  https://www.analog.com/media/en/technical-documentation/data-sheets/1930f.pdf
LAYOUT HINTS
The high speed operation of the LT1930/LT1930A
demands careful attention to board layout. You will not get
advertised performance with careless layout. Figure 6
shows the recommended component placement.

So in doubt use that.
A 20 V diode for 20 V output won't work.
What are all these vias connected to? Why don't you for starters delete all those? Or show the full copper fill you are using? The layout as shown does not make sense. You didn't answer the layer setup question - assuming it is two layer.
Verify voltage derating on ceramic caps (input and output) as explained in the datasheet.
However components "dying" hints something else is wrong here. Where does your input voltage come from? Car battery?

[zachary5577]

Quoting from the datasheet  https://www.analog.com/media/en/technical-documentation/data-sheets/1930f.pdf
LAYOUT HINTS
The high speed operation of the LT1930/LT1930A
demands careful attention to board layout. You will not get
advertised performance with careless layout. Figure 6
shows the recommended component placement.

So in doubt use that.
A 20 V diode for 20 V output won't work.
What are all these vias connected to? Why don't you for starters delete all those? Or show the full copper fill you are using? The layout as shown does not make sense. You didn't answer the layer setup question - assuming it is two layer.
Verify voltage derating on ceramic caps (input and output) as explained in the datasheet.
However components "dying" hints something else is wrong here. Where does your input voltage come from? Car battery?

Thanks for the feedback! Appreciate it.
For the layout, I did try to follow the one recommended in the data sheet.  And I agree that the 20V diode doesn't make a whole lot of sense.  I was thinking of swapping it out for the MBR0530.
All the vias are connecting ground top and bottom pours.  It is a a two layer board.  I've attached here the top and bottom copper pours.  The capacitors for this board are X5R/X7R with 50V rating.

The supply is a 12V lead acid that occasionally powers two 500gph Rule pumps.

[ArdWar]

Using 16 Vabs part for 14.8 Vin nominal is way too close for my comfort.

The supply is a 12V lead acid that occasionally powers two 500gph Rule pumps.

So there's definitely surges from pump start-stopping.

[zachary5577]

Using 16 Vabs part for 14.8 Vin nominal is way too close for my comfort.

The supply is a 12V lead acid that occasionally powers two 500gph Rule pumps.

So there's definitely surges from pump start-stopping.

This boost converter is being used in a very specific setup - typical supply should be 12V from a lead acid.  I was having trouble finding an switching IC with a higher input voltage.

However, the lead acid battery is charged either ocassionally by a lead acid bat charger (which typically supplies 13-14.8V when charging) or a solar panel. What absolute input voltage should I be looking for in this case?

Voltage source has sagged when the pumps turn on by 2 volts (from 12-10V) when not on the charger.  When the battery charger is on and the pumps turn on, the charger tries to compensate and I think raises the vin voltage up to 14.8V.  There are flyback diodes on the pumps and I haven't seen any transients when they turn off more than maybe .5V?

[zachary5577]

@ArdWar What's the issue with having a 10V Zener at Z2?

[zachary5577]

Thank you for the feedback!

1) I've removed the excess vias. 
2) I also removed Z3 (the zener across vin) and just added a large electrolytic cap on the input.  I went back an looked at the pumps when they stalled and saw that the battery voltage could jump several volts.  I tested with the electrolytic and it seems to be enough to suppress it.
3) I've replaced D1's MBR0520 with an MBR0540.

Since cermamic capacitors derate quite a bit at higher voltages, my plan is to swap out the output cap (C2) for a tantalum cap instead (maybe increase the capacitance too) and add in a cap in the feedback path to tune the stability (since the tantalum has a higher esr and it's recommended in the lt1930 datasheet). 

Let me know your thoughts and again, thank you for your time!  I'm learning a lot here.

Regards,
Zachary Anderson

[mariush]

Any particular reason you're using an expensive LT1930?  There's so many better options out there for what you want (up to 20v 250mA - 5 watts output)

For example

LM5157 : https://www.digikey.com/en/products/detail/texas-instruments/LM5157QRTERQ1/15856606  https://www.ti.com/lit/ds/symlink/lm51571-q1.pdf

MP3426 : https://www.digikey.com/en/products/detail/monolithic-power-systems-inc/MP3426DL-LF-Z/5292361    datasheet : https://www.monolithicpower.com/en/documentview/productdocument/index/version/2/document_type/Datasheet/lang/en/sku/MP3426/document_id/1125

MP3435 if you don't mind bigger inductors, as it runs at 600 kHz :
https://www.digikey.com/en/products/detail/monolithic-power-systems-inc/MP3435GL-Z/16639901 or https://www.digikey.com/en/products/detail/monolithic-power-systems-inc/MP3435GL-P/16639903

datasheet https://www.monolithicpower.com/en/documentview/productdocument/index/version/2/document_type/Datasheet/lang/en/sku/MP3435GL/document_id/9822/

[zachary5577]

Any particular reason you're using an expensive LT1930?  There's so many better options out there for what you want (up to 20v 250mA - 5 watts output)

For example

LM5157 : https://www.digikey.com/en/products/detail/texas-instruments/LM5157QRTERQ1/15856606  https://www.ti.com/lit/ds/symlink/lm51571-q1.pdf

MP3426 : https://www.digikey.com/en/products/detail/monolithic-power-systems-inc/MP3426DL-LF-Z/5292361    datasheet : https://www.monolithicpower.com/en/documentview/productdocument/index/version/2/document_type/Datasheet/lang/en/sku/MP3426/document_id/1125

MP3435 if you don't mind bigger inductors, as it runs at 600 kHz :
https://www.digikey.com/en/products/detail/monolithic-power-systems-inc/MP3435GL-Z/16639901 or https://www.digikey.com/en/products/detail/monolithic-power-systems-inc/MP3435GL-P/16639903

datasheet https://www.monolithicpower.com/en/documentview/productdocument/index/version/2/document_type/Datasheet/lang/en/sku/MP3435GL/document_id/9822/

We went with the LT1930 for a few reasons:
1) We have a working simulation of the circuit in LTspice
2) The exposed leads make it easier to work with (the chips you share a flat packed)
3) There are thousands of these chips in stock (less likely to go out of stock)
4) The footprint matched the previous IC that was there

On another note, I can see that tantalums are probably not what I want on the output since the switching frequency is so high.  So I suppose it's best to stick with ceramics (maybe 2 1206 10uF 50V rated X5R caps).  Or perhaps a tantulum in parallel with ceramic but I'm not confident that makes much sense in terms of ripple.

[trobbins]

That bottom layer image is difficult to discern due to the colour contrast, and both layer images have text that can't be read as it sits above tabs etc.  Do you also have a top-side photo/image showing parts layout on the pcb?

Does the PV panel have a regulated output and is it directly connected across the battery?  The concern is to avoid excessive voltage being applied to pcb (eg. from low-temp, high sun, light load conditions on the PV panel).

[Dr_Neoo]

I would focus on making the output loop smaller. One easy way would be to move C2 inside of the VOUT trace going up to the feedback resistors. I would also recommend adding at least one more output capacitor in parallell.

Do you have any EMC/EMI requirements on the design? If you do consider adding a filter in series with the output.