TPS65131 split rail power board

[Skimask]

Working on a new board...new to me...  Built it up using a homemade QFN20-DIP adapter board.  Worked, but not all that well, likely due to the lack of a halfway decent ground plane.

TPS65131 in a QFN20 package, 2.1" x 1.85", flood filled with ground on top and bottom, traces that handle any sort of load are fattened up, stitching vias here and there for both ground and those same load traces as well as a few doubled up traces on the bottom layer for a bit more current handling capability, fatter vias for extra hookup wires on various signals, 2 thru-hole trimmer pots for adjusting + and - outputs.  I've got silkscreened notes on the bottom layer.  I hid those in the bottom layer picture for a bit of clarity.

Input at the bottom, 2.7V-5.5V, single cell Lipo, USB, etc.
Outputs at the top...
Positive output on the top/left, adjustable from Vin+.5v to ~15V, ~350mA max @ ~+15V output with 3.3V input
Negative output on the top/right, adjust from -2V to ~ -15V, ~150mA max @ ~ -15V output with 3.3V input
Jumpers to selectively enable the positive and negative outputs, as well as the 'power save' mode which enables pulse skipping at light loads (increasing efficiency).

Looking for any more good ideas.

[ThomasDK]

Looks like you have no solder mask between the qfn pins. You might want to adjust your solder mask expansion.

Also, the fat ground connection going through multiple pads might become difficult to solder properly.

Thomas

[tszaboo]

The trick for a good SMPS layout is to reduce the loops where the switching current flows. So you want the inductors, and the capacitors and the extra FET as close to the chip as possible. I think you can improve this layout. Dont restrict yourself to 90 degrees, you can play a little with the orientation, that usually leads to a better result. Look at the datasheet layout example.

[Skimask]

@Thomas - Solder mask, true.  Going to use OSHPark, used them before, not sure if that service can handle that small of a sliver of mask between the pins.  Won't hurt to adjust and try.  Worst case I have to break out the X-acto knife and scrape some away when I get the boards in hand.
Fat ground connection?  Which one?  All of them?
Thinking I should use the 'thermal' option when doing the polygons rather than not?
EDIT:  I checked the mask.  There is actually a gap between the pads on the QFN, but it's only .002".  I think I can fatten that up to .004"  Might be below their capabilities but still get a little something in there.

@NANDBlog - The "factory" eval board layout and the layout in the datasheet both use primarily 0402 parts (except for the fat caps which are mostly 1206).  My eyes aren't that good any more, even though I've got a decent Amscope   ...which is why I went with 1206 lands vs. 0402.  The QFN20 is gonna be bad enough!
I'm not too far off the eval board layout as the eval board is a fair amount larger than what I threw together.  According to the datasheet, Everything has to be close to the chip.  But...point taken.  I'll see what's what.

Just so I'm not missing anything here...
Redid the screenshots so the GND fill is highlighted.
Don't suppose you could highlight what you think might be a 'bad' ground loop?  Maybe?  Maybe not?  I mean, I know what a ground loop is and how they're directly affected by frequency...but...I'm also not a professional switch mode power supply designer by any stretch of anybody's imagination...

[tszaboo]

I was not talking about ground loops, but current loops. They look something like this: Switching output of IC -> inductor -> Diode -> capacitor -> ground of capacitor -> ground of IC. Follow where the high frequency current goes, the less it travels, the better.
But now that you mentioned it, your ground needs some change also. You want to avoid what you did at those 4 vias close to each other (bottom side). There should be a short path between the IC's ground connection, and every other ground connection of the board. If they have to travel a lot, that is bad. Just by moving some traces, I think you can improve this.

[Skimask]

I was not talking about ground loops, but current loops. They look something like this: Switching output of IC -> inductor -> Diode -> capacitor -> ground of capacitor -> ground of IC. Follow where the high frequency current goes, the less it travels, the better.

Gotcha.

But now that you mentioned it, your ground needs some change also. You want to avoid what you did at those 4 vias close to each other (bottom side). There should be a short path between the IC's ground connection, and every other ground connection of the board. If they have to travel a lot, that is bad. Just by moving some traces, I think you can improve this.

Talking about the 4 vias, kinda placed vertically (in the picture) with a slight 11'o'clock slant to them?  Those are just enable/disable inputs, no freq's on those.
But I get your point about how the current for the negative switching kinda has to go around those vias to get to where it's gotta go.

EDIT:  Yes, I see some looping going on now.  For one, the negative rail inductor, L2, it's ground current has to go all the way around those enable/disable jumpers on the right, or take a convoluted path from the left.  Since those jumpers are 'only' pullups/pulldowns for mode selection, I don't need that thick Vin rail on those.
I'm smelling what you're cookin'.

[Skimask]

Jockeyed the pieces/parts around a bit.  Short of going with smaller parts (again, don't think my eyes are up to the task any more), the PCB is a bit smaller, the parts crammed a bit more together, and the major current loops are a bit shorter...I think.  Maybe if I went with 0805 or 0603 parts, the layout would be a bit better, but 0402...not in the rest of my lifetime.
Grounds are highlighted in both pictures.  Flood fills for those same major current runs/traces.  Decided that I don't really need the jumpers and adjustment pots to be in the perfect place so long as they work where they're at.
I'm still going to add a handful of stitching vias here and there, maybe run a couple of extra traces on the bottom layer to double up on the big traces from the top layer.  Figured I'd keep the excess mess out of the way for now.

[Skimask]

I could sit here and adjust the PCB for the next few weeks or just go ahead and order it up.
Think I'm gonna go with option B and see what happens.

[Skimask]

Went ahead and ordered 3 of each.  Hope they work as decent as they look...'cause they look good enough to me.  Going to have about ~100 or so made.  Only need 30.  Keep a few for myself, put the rest up on tindie after I verify everything works as they should.

First up is the TPS65131 board, Buck/Boost/Inverting/Split-rail converter.
2.7V-5.5V In, adjustable + and - outputs.  The datasheet has all the gory details.
http://www.ti.com/lit/ds/slvs493d/slvs493d.pdf

Second is the TPS6300x (TPS63000 adjustable, TPS63001 3.3V, TPS63002 5V), Buck/Boost converter.
1.8V-5.5V In, adjustable or fixed outputs.  Again, see the datasheet for the details.
http://www.ti.com.cn/cn/lit/ds/symlink/tps63002.pdf

[Skimask]

Well...the first 3 boards, not too bad at all, at least with ~100mA loads on each rail.  I've got a big ol' box of power resistors...somewhere...  All I could scrounge up was a pair of 82 ohm 1% 10W and 20ohm 1W resistors.  Go figure.
All 3 boards ended up with more or less equal results, down to at least 2 digits anyways.  I average the 3 results into one.
The disparity between the voltage and current readings at the DP832 vs. a BK2709B/uCurrent is a bit concerning though.  I figure the current disparity might be due to the uCurrent's bandwidth.  Got no idea what the deal is with the differing voltage readings though.

PCB     PCB
V(in)   I(in)   W @ PCB   DP832 V(in)   DP832 I(in)   DP832 W   V+ Out   I+ Out   + W Out   V- Out   I- Out   - W Out   Total W   Total Eff.   Diff DP832 vs PCB W   Diff DP832 vs PCB V   Diff DP832 vs PCB I
4.994   0.538   2.687     5.030          0.610          3.068   10.400   0.117    1.217     10.050   0.083    0.834     2.051     0.763          0.382               0.036                 0.072
3.995   0.621   2.481     4.040          0.790          3.192   10.290   0.117    1.204     10.050   0.084    0.844     2.048     0.826          0.711               0.045                 0.169
3.003   0.841   2.526     3.060          1.080          3.305   10.060   0.115    1.157     10.040   0.085    0.853     2.010     0.796          0.779               0.057                 0.239
2.602   0.902   2.347     2.660          1.100          2.926   9.980    0.114    1.138     8.620    0.072    0.621     1.758     0.749          0.579               0.058                 0.198

The efficiency numbers semi-sorta-kinda match up with the datasheet, in that my circuit always calculates out to about 5% lower than the datasheet value.  One issue I know is a problem is that I've got the adjustable feedback potentiometers hanging off the board with an inch or so of wire.  I had bought a handful of 3 pin PCB mount trimmer pots...at 100 ohms instead of the 100K that I wanted!  DOH!!!  So there's some high frequency noise right there I'm sure is killing off a bit of efficiency.  Tried it out briefly with a pair of 20 ohm resistors on each output, pulling 500mA thru each rail, drawing about 2.8amps off the DP832.  Worked just fine, resistors got scorching hot, gave it up until I get some beefier resistors.  Little buggers were up to 160F by the time I got the FLIR on them.

So, the main issue...the disparity between the DP832 output readings and the BK2709B/uCurrent readings at the PCB.  I didn't see any measurable V drop in the leads feeding power to the PCB, yet the DP832 was always reading at least 36mV higher than the V at the PCB.  Same with the current.  I've got the DP832, not the DP832A so I don't get down to mA readings.  The DP832 output current read at least 70mA, and as much as 240mA higher than the current measured with the uCurrent inline with the power leads.

Looks like it's about time to pick up a couple of known, accurate, calibrated voltage & resistance standards.

All in all, 74% for 3v in and +/- 10v out, not too shabby for a homebuilt.

EDIT:  Forgot to add some notes about noise on the output rails...
The positive rail has about 400mV of noise on it at !10V @ ~100mA output, whether it's in 'Power Save' mode or not.  The negative rail, loaded the same, shows about 150mV of noise.
If the trimmer pots don't fix some of that noise (eg. removing the 1 turn potentiometers hanging on by wires), I've got 4 4.7uF 1206 SMT caps on each output rail.  For grins, on each rail, I'm going to take 2 of those 4.7uF's, stack them on top of the other 2, add a .1uF and a .01uF, and see what happens.  And if that doesn't do me any good, maybe the trimmer pots themselves might be inducing some parasitics into the feedback loop.  Maybe try replacing the trimpot with fixed resistors...lock it down and see what happens.

.......A lot of "see what happens" going on here.......

[andyturk]

I'd be interested to see how your TPS6300x boards work too. I built a little breakout board similar to yours but haven't actually benchmarked it.

[Skimask]

The biggest pain was setting that VQFN.  I did it with hot air (858D style air gun) and touched up the 'pins' on the side with a tiny chisel tip.
Built a reflow oven awhile back, SSR for power switching, PIC for control, etc.etc.etc.  Standard stuff.  Haven't had the balls to plug it in and let the smoke out of something yet.

I screwed up the initial 3 TPS6300x boards.  Didn't have the correct PCB layout.  Used an MSOP10 package.  Looked close.  Not close enough...Not narrow enough.  Fixed that.  Got another batch coming from OSHPark sooner or later, probably late this week if their manufacturing and shipping times hold steady with what I've gotten in the past.  If you think you're good enough to solder wires straight to those TPS6300x VQFN chips, I'll send you the 6 'broke' PCB's I've got.  My eyes aren't good enough for that anymore.

(I'm adding some more info to the earlier post regarding noise)

[andyturk]

My first attempts at soldering the VQFN failed, but I think that was down to using cheap paste. It worked after I cleaned off the board and tinned the pads using a regular iron and then used hot air (with liberal flux) to reflow the chip. For a cheap-n-cheerful double sided OSHPark prototype, it seems to work well.

[Skimask]

Same here.  I didn't tin the pads first time around for some unknown brain fart reason.

Looks a bit like the demo board PCB.  I went that direction first time around.  Wanted more "options" on the board after I got to thinking about it...enable, power save, ability to use all 3 (TPS63000, -1, -2), etc.

[Skimask]

Got the TPS65131 PCBs built up.  Testing them out.  Getting a lot of noise on both positive and negative output rails.  Not sure what the best route to take from here to reduce the noise to a more manageable level.  Sure, I could go in there, waste my time, and start swapping out cap's, adding inductors, etc.  I'm betting somebody smarter than me might be able to point out a single point of failure on my part.

The output noise may or may not be a factor anyway as I plan on using a pair of linear regulators to knock the outputs down to +/- 11.5v for use with an AD7367 ADC.

I'm using a single load resistor for these tests, 82ohms, and set the output voltage to about +/- 14.5v on each rail, contrary to what I mention in the video, which loads down each output rail with about 177mA.
At these loads/voltages/etc., my calculations show about 63% combined efficiency between the two outputs.  About 10% lower than what the datasheet graphs show.  Close enough for me.  Get rid of some of the noise, the efficiency will likely go up.

EDIT:  I already see one problem.  The via on the VPOS rail to the left of the positive catch diode.  It's not filled and it's cutting off most of the VPOS rail coming off the diode!  Well...that can't be good!  Same thing with the via on the other side between the positive catch diode and the TPS65131.
Jeeze...there's a newb mistake right there.

[Skimask]

Thought about it overnight...and had some DUH thoughts.
There's ~29Khz ripple on the output and the input.  Feeding the whole thing from a DP832 with those 3ft long leads with what appears to be about ~50mV drop.  That's probably no good.  Get rid of that ~29Khz ripple and the overall noise has to go down.

On the PCB, I've got a single 4.7uF cap across the input rail.  I soldered up a 120uF cap on the back side and a .1uF cap across the input wires as well.
In addition, I put 2 .1uF caps stacked on top of 2 of the 4.7uF output caps on each rail, for a total of 4 (2 on each rail).

Without the extra cap's noted above, I was getting about ~1.5v of ripple at the input.  With the cap's added, input V ripple dropped to about 350mV, and the freq of that ripple dropped from ~29Khz to about ~26Khz.
Output didn't change much.  The freq of the main ripple on both positive and negative outputs still matches the input ripple, about ~26Khz now.
The positive rail ripple on that ~26Khz wave dropped from ~500mV to ~420mV.
The negative rail ripple didn't change much except for the freq.  The majority of the ~26Khz ripple is gone, and the bulk of what's left is due to the switching spikes at ~1.3Mhz, roughly ~160mV now.

Going to mount an 18650 in the holder and see what happens.  Still haven't done this yet.

[Skimask]

Still working on the TPS65131 board...trying to get a clue.
Attempting to use the TPS65131 to get +/- 15V (give or take) from a single 18650 Li-Ion cell.

A bit of my schematic explanation


And some action while in operation.  Major change from the first video is the removal of the TP4056/DW01 Li-Ion charger/protection board, thinking maybe it was the cause of the input voltage ripple.  Not this time.  Not a thermal problem as it the issue occurs immediately after start up on a cold chip.  Nor is it a power supply problem as far as I can tell.

I've powered the board from a variety of combinations: DP832 thru the TP4056/DW01 charger/protection board, single 18650 cell thru the TP4056/DW01 board, single 18650 only, DP832 feeding 4V directly into the 18650 (taking care not to overcharge it).
In addition, in the 3rd video, I've got each rail loaded down to ~150mA.  That's a bit above spec for the negative output rail, but the negative rail is the one that's performing correctly.  It's the positive rail that's screwing up horribly.  One thing not shown in the video is removing the extra loads and only pulling about 20mA from each rail with TPS65131's power save mode enabled and disabled.  Same results on all tests.


Looking for a better clue.  'cause I'm out of them.

[Skimask]

Figured it out.  I think.  Tried the fix at low output voltage, low output load.  Trying next at max volts/max current next.

Update sooner or later.

  Dumb fix too 

[Skimask]

Fixed...
I'm a pinhead.
When putting the PCB together in EAGLE, I swapped the values for C5 (boost converter compensation cap) & C6 (positive feedback snubber cap).
C5 (compensation) should've been 10nF.  C6 (feedback) should've been 6.8pF.  Compensation isn't going to compensate for shit with a 6.8pF on it.

https://www.youtube.com/watch?v=HOYff4N6mVo&feature=youtu.be

Happy guy...