New switcher - causing issues!

[Wilksey]

Hi Gurus!

Attached is a PSU that I am trying to get to work, datasheet for the chip here:
http://www.farnell.com/datasheets/1747276.pdf

I have pretty much copied the reference circuit from page 10, just adjusted the FB resistors for ~4V.

This is the second chip that has decided it will stop working for no apparent reason, the first one just died, no output, nothing!
Second one worked for a bit, I had 3.9V on the output, and 0.78V on the feedback, so to be expected, going into the 3.3V regulator, which remains fine, I can feed 5V into the test point and get 3.3V reliably out of the LDO.
The buck decided to adjust it's output to 2.3V to 3.2V randomly, now it is dead, 0V on the output, I have tried changing the inductor, and the caps, tried electrolytic and ceramic, makes no difference.

Current wise, the 3.3V rail has a PIC24 connected to it, which works fine, checked the outputs, the board itself has no shorts, the PSU draws 30mA @ 12V, the 4V eventually will go to a GSM chip, but this is not connected, so the only thing on the buck output is the LDO.

I have designed other switch regs in the past with no issues, these we ~50p on Farnell, should have known better!

Can anyone see anything obviously wrong with the attached circuit, specifically why the chip would fail.

TIA!

[georges80]

More likely your PCB layout - got a picture of the layout (all layers)?

cheers,
george.

[Wilksey]

Hi George,

Thanks for the reply,

I have attached pictures of the regulator section board layout, just 2 layers, mostly top copper, I have omitted the ground plane for clarity.

I have laid out boards before with switchers on and they have all been fine, this one is a bit odd!

TIA!

[kony]

Board preview wihtout poured planes shown serves no purpose - I almost started ranting, then saw the note in post. Please show PCB layout in as-is fashion.

[nctnico]

Even with pours the ground loop is probably way too large. I'm inclined say its all wrong because the feedback circuit is in the way of creating a small loop for the ground return currents. Check some layout recommendations from TI or National for optimal component placement for such a circuit.

[DanielS]

I agree with nico, the ground and signal loop in the feedback network are far too large, this cannot be doing you any good. You should also be tapping your feedback signal from one of the output filter capacitors, not right off the inductor, otherwise you end up adding trace inductance , resistance and switching noise to your error signal when what you want is the filtered output voltage. I would tap the feedback trace from the second capacitor and snake the trace between the first capacitor's pads.

[homebrew]

Two things that I would add:

1) The electrolytic capacitors might be problematic by themselves. The datasheet recommends to use MLCCs. They specify to use 2x C3216JB1C226M which I would stick to or replace them with X7R caps in the first place.

2) The datasheet also recommends to connect the thermal pad to a ground plane using some vias. You could easily put 5 vias (0.3 mm) under this pad. If using ground planes on both sides, stitch them together with vias.

3) Your input traces are quite large (which is totally fine) but it gets VERY dense at the pads. Is this really still compatible to your boardmaker's design rules?

[Wilksey]

Hi,
Thanks all of for your replies.

The feedback pin stays at 0.78/0.79V, but the output voltage changes, input stays the same.

I tried replacing the 22uF electros with multi layer ceramics but it made no difference.

The ground of the feedback circuit is connected almost opposite the power input pad, so it doesn't have that far to go?
There are quite a few GND via's around to connect various points to the GND plane on the bottom, there is no top plane.

Yes the components could be tighter, and I could try cutting the track and moving the feedback to the end of the output caps

I could understand if the supply was unstable, but what could cause it to give 0 output suddenly?  The input is fine, the chip itself doesn't even get warm, the thermal pad is not connected to the ground admittedly, but there is a thermal pad and I have reflow soldered it before soldering the chip pins to make sure it is connected.

I presume something is blowing the chips, but I can't see what would, the output also goes to a FET which is not fitted, I have checked for shorts, the PSU doesn't dip or short when the output goes dead.

[hamdi.tn]

PCB layout and Ground with DC/DC switcher are important, however i did a lot of prototype with buck chips and bunch of wires not even a proper pcb. chip react poorly but it do the job for a quick test.still you have to reconsider your layout  ! . i think like homebrew said , capacitor are important too, low ESR cap are a must.

[georges80]

Where is the ground plane layer? Please post it. I assume then that this is a 4 layer board since you mention that you're only showing the top/bottom layers?

Show us the ACTUAL layers as flooded etc (all of them).

cheers,
george.

[Wilksey]

Hi George,

The bottom layer is the GND plane, I removed the GND plane for clarity, the board is indeed 2 layers - top and bottom.

Apologies, I should have included the image with the GND filled.  This is now attached.  I've removed the top copper again, for clarity.

Thanks

[c4757p]

That's quite bad, look at the current path between the input cap and the output cap.

[georges80]

Yeah, you have a huge cut ground plane with that trace running from TP1 - can't be good...

Please show the vias from the top layer (e.g. to the in/out cap grounds) going to the ground flood.

What I'd like to see is the complete Top and Bottom layers - with traces/floods/vias etc.

cheers,
george.

[Wilksey]

The plane is cut, but the ground is routed on the top layer for that chip, not the bottom layer.
I tried to keep the ground path for the chip relatively straight and point to point.
The caps do not go through vias, but directly to the GND pad on the top layer (as shown in previous post with top and bottom layer) where the GND connection is soldered to on the top layer.

[georges80]

Please, post the top/bottom layers, showing traces/floods and vias.

If you have all the vias shown, then there's really minimal connection from the output caps to the ground plane other than a long trace and that's not a good plan.

cheers,
george.

[rx8pilot]

The layout, as others have said, is not going to work. The layout details are AT LEAST as important as the components you put on it. I learned these lessons the hard way.

Notes that others have not yet mentioned:

PGND and AGND are different for a reason. They need to be tied together at a single point. The idea is to keep the inevitable high current/voltage (di/dt and vi/vt) switching noise from impacting the FB and COMP pins. The FB divider should be very close to the FB pin and be surrounded by the AGND if possible. The same goes for the COMP components.

The current path from IN to OUT should be as short as possible. PCB inductance is deadly and it only takes tiny amount of it to destabilize the circuit.

I seriously doubt there is anything wrong with the parts you have. The layout of a switcher, even a simple one like this, is nearly a black art. Just getting voltage on the other side with a DMM does not mean it is working right. It only means that it is doing something. To know if the circuit is behaving as designed, you have to at least have a scope and the delicate skills to measure your circuit. I spent a ton of time just learning how to measure an SMPS and get basic performance information. It took even longer to learn the details of layout. I read a lot, experimented a lot, and the looked at known good examples. The examples were invaluable at cluing be into what was wrong.

There was a design that I did that was too noisy. I purchased the dev board from TI and saw that they had a rather quiet design, so I hunted for the differences, some of which seemed so insignificant. Sure enough, my next revision was fantastic - step response, PARD, ripple, regulation, efficiency, etc.

Dont give up, but also don't think that an SMPS is something you slap on a PCB and go. They are sensitive little devils that mix fast current switching right next to super sensitive analog controls. There is no forgiveness.

[Wilksey]

Hi George,

Apologies, Is this what you wanted? An all-in-one view?

On the far left, there are pads 3 and 4 shown as GND and VIN, this is where I have soldered 2 wires directly and connected the 12v PSU.

Thanks

[Wilksey]

Hi RX8Pilot,

I have used different switchers in the past and put a few on perf board, they may not have been ideal, or worked 100% efficient, but they have worked, I have never had any other chip perform like this one.

AcHmed99,

I recalculated the components for 4V rather than the values supplied in the DS.  The output voltage went from 3.9 to around 3.7 down to 3.2 down to 3.0 down to 2.8 then to 0, all in the space of a minute or so, it didn't give me chance to hook a scope up before it died, nothing measures short cct, just 0V on the output pin, the FB pin stayed around 0.79 (0.8 it should be), the 12V PSU was drawing around 30mA, do you think it could be not enough load? I must admit I didn't think of that, I could add a load to see if it works better?

My main wonder if you will is why the output has gone to 0V, if I set the bench supply at 4V and stick it on the VOUT TP it works absolutely fine, I am sure the components are fine, and I have more than likely messed up, which I don't mind , maybe on my other layouts with SMPS chips I have just been lucky, I try to make the main PSU components continuous if I can, I am no expert at PCB design, I know enough to get by usually.

If I redesigned with the LM2576 or something it would have probably worked fine first time, but I am now curious as to what I did to make the chip feel like not working.

[Wilksey]

Hi Blueskull,

Two short (1 or 2cm 16/0.2mm) wires were used, PSU was powered up first to check voltage, powered off, GND connected then 12V, PSU turned on, subsequently the PSU was then just turned on thereafter.

The chip was stone cold, I checked the power rails for shorts etc and found none.

[Monkeh]

Hi RX8Pilot,

I have used different switchers in the past and put a few on perf board, they may not have been ideal, or worked 100% efficient, but they have worked, I have never had any other chip perform like this one.

How fast a switcher have you used before?

I have blown up a number of 600kHz switchers with poor layout (actually, the external FETs, they're quite high power). Your layout is not workable for these frequencies.

[georges80]

The ground connections are quite weird/horrible. Your output caps only go to ground via the long traces and not to the plane.

Analog small signal stuff (compensation, feedback etc) need to be over 'quiet' ground areas.

Some switchers can be hobbled together on perf board, some on 2 layer boards and some NEED 4 layer boards. I work with switchers all the time (though mostly constant current for LED drivers) and I have a few designs that will NOT work with 2 layers.

Attached is an example proto of a 3.3A LED driver. I used some copper tape to create the ground plane and the switcher IC has a thermal pad and PGND connections that solder to the copper plane. You can see how I've soldered the caps to minimise ground loop/path length etc. This was thrown together to test a new switcher chip before I get prototype PCB's fabricated.

Anyhow, I'd safely bet that you have primarily a layout issue with your design versus component issues. I've used ceramic caps with long leads into buck and boost LED drivers and no issues. Concentrate on your layout an THINK about where the current flows in your various paths. Consider the Feedback signal (critical) and where noise can couple in due to ground noise and ground offset issue (high currents in long paths will create voltage drops). Consider noise around the compensation pin and components AND the noise on its ground.

Sometimes ONE ground for everything (power and signals) will NOT be a good thing.

cheers,
george.

[Wilksey]

Hi RX8Pilot,

I have used different switchers in the past and put a few on perf board, they may not have been ideal, or worked 100% efficient, but they have worked, I have never had any other chip perform like this one.

How fast a switcher have you used before?

I have blown up a number of 600kHz switchers with poor layout (actually, the external FETs, they're quite high power). Your layout is not workable for these frequencies.

I have used a TI TPS6 part before which runs at 1MHz I think from memory, two LT parts, which I think were 0.5 / 1Mhz parts, a LM2676 which is 60 odd KHz I think.

George,
Are you saying that it would have been beneficial to have connected the ground connection to the plane?

I am wondering if it has anything to do with the analogue ground being connected with the digital ground, I can't see anything about isolation on the DS, but do they need to be isolated?

I must be honest I am quite ignorant when it comes to frequencies, not on purpose, but I try and make the connections as direct / short as possible, sometimes they are bit longer than they perhaps could be, but usually I can get away with it.

[georges80]

The output caps etc should definitely go to the main power ground (same as the thermal pad of the switcher). You need a quiet ground for the comp circuitry and under the feedback trace etc. The quiet ground would be a cut area that current doesn't flow through (i.e. the ground currents that the main in/out caps connect to and your load).

Create a good ground to tie the input/output caps together and directly to the switcher IC PGND. That is job #1. Then create the cut ground that is quiet (analog ground). Think about where the compensation circuit connects to and also the feedback trace etc - i.e. NOT over the noisy power ground.

I'd rearrange your circuitry if needed to achieve the ground goals. Fatter traces to/from the inductor and as short as possible. Don't route feedback etc need the inductor and certainly not under it etc.

Read the datasheet where it talks about the layout, it's not very details and unlike other manufacturers there's not even a recommended layout, but at least there's some hints.

Unfortunately some switcher IC's are easier to use than others. In the near MHz frequencies, many can be very 'tricky' to get running stable an efficiently.

That's about the limit of my suggestions since I've never used that part and don't know how finicky it is.

cheers,
george.

[T3sl4co1l]

Flood both sides with ground, and stitch heavily with vias.  Such construction can save a lot of bad routing, of course you should be doing that well in the first place.

Tim

[Wilksey]

Hi George (and others)

I do appreciate the tips and hints!

It's the first time I have used this switching reg, and it will probably be the last!  I will probably stick to TI or LT parts, at least they work with my bad layouts

If anyone has any more feedback / info as to why the switcher may have just died I would still be very interested to see what thoughts are!

Thanks