What's the 'best' way to get bipolar power from a wall-wart?

[plushterry]

If your 5.6v zeners are shunts then you need to consider there is a TDP and current limit before they pop. Then you would have no protection as a result of going over voltage. Do an internet search for power supply crowbar circuit. But this may not be needed if your 5v DC supply has some over voltage protection or some very predictable failure mode of catch fire and turn off.

yeah I've been considering a crowbar. It seems a bit brutal. I suppose you get instant feedback that somethings wrong (gadget wont turn on) and it doesn't 'hide' the problem initially, like shunt zeners would.

The problem I was trying to solve was overvoltage/spikes from the correct adapter. The diodes I've specced have 1W power dissipation, with 2 in parallel which should allow for a volt or so over for extended periods.

Now you're making me think about it, I will put a crowbar in. I am the end-user, so best make it fairly robust

[EATyourGUITAR]

This completely depends on what you know and what you trust about your 5v adapter. If it is sealed then you can't look at it. If there is a datasheet that says it has over voltage protection then you don't need the crowbar. You can model what it would take to shunt more than 1W or 2W for 30 seconds. If you have 15v for example with an output impedance 10 Ohms that gives you 1A over 5.6v for 5.6w. it all depends on what over voltage you get when things go bad and what is the output impedance of of the 5v supply and what is the duty cycle when it starts going into failure. At 2w you can sustain 9v for 30 seconds with no airflow IF your output impedance is 10 Ohms. If I were you I would let it burn the zeners or the SMPS. I wouldn't worry about it too much because the SMPS can be replaced, the synth circuit can be replaced. Your not selling it and the risk is low. PTC fuses are cheap. You can look at that also. The good reason to do a crowbar would be that you can teach yourself electrical engineering on a real project and you can get a job later with what you learned. Some people do it for fun.

[plushterry]

OK, so I've been back to the drawing board, overhauled my design quite a lot.


I've selected a different switching chip, the LT3471, which seems to be better all round. Higher max Vin, higher output current, smaller footprint and lower cost. Also it allows higher Vout than the TPS65130, so I can allow for the dropout voltage of the "LDOs" and still get +/-15V at the final output.

The max Vin for this chip is 16V, with an operating range from as low as 2.4V. I've put a 15V crowbar which will allow DC adapters in the 5-12V range for power source.

I decided against using a polyfuse, going for a conventional slow-blow type instead. I think it's better that there's some consequence for doing something stupid like plugging in the wrong adapter.

The regulators I was using in the previous design were super low-noise types and would have been getting close to their sensible limits with regards to current draw. It seems to be quite tricky to find negative regulators that were suitable so I went for a combo of MC79M15/MC78M15. The result is higher current handling capability and lower cost at the expense of greater noise and higher dropout voltage. I put "LDO" in quotes because the dropout is 2.2V at 500mA on the positive regulator, not exactly low compared to some other devices.

I think this a better solution than before, but as always if anyone can see anything stupid i've done, please feel free to talk some sense into me

[MikeDB]

Not sure why the datasheet doesn't suggest it, but since you have a Cuk convertor on the negative output so have sourced a coupled inductor, odd the didn't suggest a SEPIC on the positive using the same inductor as then both sides would be pretty clean even before the regulators. (Nothing with a 78 or 79 in it can be called an LDO :-)

[plushterry]

Not sure why the datasheet doesn't suggest it, but since you have a Cuk convertor on the negative output so have sourced a coupled inductor, odd the didn't suggest a SEPIC on the positive using the same inductor as then both sides would be pretty clean even before the regulators. (Nothing with a 78 or 79 in it can be called an LDO :-)

Ah. well, I did source a coupled inductor, but the were going to cost me nearly 2quid each and I couldn't find any in the fabricators part list (meaning i'd have to put them on myself) so I opted for a pair of separate inductors which are 15cents a piece (at the expense of some efficiency).


I managed to find plenty of LDOs with ~100mA outputs but finding anything between that and an amp (particularly a negative one) wasn't easy

[MikeDB]

Ah. well, I did source a coupled inductor, but the were going to cost me nearly 2quid each and I couldn't find any in the fabricators part list (meaning i'd have to put them on myself) so I opted for a pair of separate inductors which are 15cents a piece (at the expense of some efficiency).

I managed to find plenty of LDOs with ~100mA outputs but finding anything between that and an amp (particularly a negative one) wasn't easy

Hehe - sounds like you use the same fabricator as me. If you're not using coupled inductors then the capacitor does take far more of a hammering than those in the bypass positions so it's best to split it up into several smaller ones in parallel to get the same capacitance, and use large exposed areas on the PCB to dissipate some heat.

[plushterry]

Hehe - sounds like you use the same fabricator as me. If you're not using coupled inductors then the capacitor does take far more of a hammering than those in the bypass positions so it's best to split it up into several smaller ones in parallel to get the same capacitance, and use large exposed areas on the PCB to dissipate some heat.

I take it you mean the 1uF in position C5 on my schematic?

Thanks for answering my questions! much appreciated

[MikeDB]

Hehe - sounds like you use the same fabricator as me. If you're not using coupled inductors then the capacitor does take far more of a hammering than those in the bypass positions so it's best to split it up into several smaller ones in parallel to get the same capacitance, and use large exposed areas on the PCB to dissipate some heat.

I take it you mean the 1uF in position C5 on my schematic?

Thanks for answering my questions! much appreciated

Yes - I just added a schematic above showing the capacitors split for both SEPIC and Cuk convertors.

[plushterry]

Yes - I just added a schematic above showing the capacitors split for both SEPIC and Cuk convertors.

Thanks Mike!

[v8pete]

Some of those high switching frequency regulator ICs can be an absolute pig to get working reliably. We used a Linear Tech part in a project about four or five years ago, an inverting buck-boost IC, internal Mosfet & low external component count, just the single inductor, to produce a -12V rail from a 48V DC input. Our circuit was basically almost an exact copy (...and in desperation, eventually became an exact copy) of LTs demo board for this part. The problem that we had was that it would power-up ok about five times in a row, then on one of the next few occasions the internal Mosfet would go dead short. We used the exact same brand and part number of inductor as the demo board (didn't want to run into weird saturation or parasitic problems), and I spent ages pouring over our layout, which was also sent to LT in the US for review. Nobody could find the problem. The demo boards however, worked fine & you could even take off a lot of the various bypass caps & it was impossible to make it fail. We never found out the cause & ended up re-spinning our board (which was a big data acquisition PCB) using a different part (that solved the problem). Maybe we had a dud batch of parts, but that seems unlikely, since the vendor sent us quite a few more during the time we were having our issues.

I still have a demo board somewhere; will see if I can dig it out to check the part number. This was about the only occasion that I can honestly remember in my whole career to this point where we had no real idea what the hell was causing the problem.

[MikeDB]

One possibility is your primary inductor had a shorted turn. That will kill the IC like that.

[v8pete]

One possibility is your primary inductor had a shorted turn. That will kill the IC like that.

Yep, we built more than one board and they all did the same thing. Reminds me of the days when you'd diagnose shorted turns in colour TV line-output transformer secondarys by placing your hand on the outer winding - remembering to switch the set off first!

i'll try and find the demo board as I'm curious to know if the part is still in production & if others had issues with it too.

[MikeDB]

One possibility is your primary inductor had a shorted turn. That will kill the IC like that.

Yep, we built more than one board and they all did the same thing. Reminds me of the days when you'd diagnose shorted turns in colour TV line-output transformer secondarys by placing your hand on the outer winding - remembering to switch the set off first!

i'll try and find the demo board as I'm curious to know if the part is still in production & if others had issues with it too.

What was the IC number ? One thing I'll say is the quality of evaluation boards varies wildly. One TI example layout omits one of the most critical tracks so you have to add it in up and down through vias !

[v8pete]

What was the IC number ? One thing I'll say is the quality of evaluation boards varies wildly. One TI example layout omits one of the most critical tracks so you have to add it in up and down through vias !

Can't remember off hand Mike, but I'll have a look for the board..I think I saw it a few months ago whilst rummaging through some old stuff. I do recall that there were definitely some discrepancies between the data sheet and the dev. board schematic (I think we ended up trying all practical combinations of everything!)

[skee]

Looks like you’re not going down the MFOS route, but FYI for anyone considering it, the recommended 500mA wall wart may not be suitable for some applications, due to significant voltage droop on loads much over 200mA. This can pull the unregulated voltage supply below the drop out level of standard regulator ICs.

I have just replaced mine with an RS 1.5A version, which has restored the unregulated side of the psu, and significantly improved stability overall.

[MikeDB]

I have just replaced mine with an RS 1.5A version, which has restored the unregulated side of the psu, and significantly improved stability overall.

I'd second using the RS power supplies. I specify them all the time. They are more expensive than others, often double, but I trust the approval labels on them and they seem far more up to most jobs, running noticeably cooler.

[plushterry]

Some of those high switching frequency regulator ICs can be an absolute pig to get working reliably.

thanks for that Pete!

[plushterry]

Here's the layout I've come up with. I'm pretty pleased with it, but i'm sure it's not perfect.

I watched a few videos with Rick Hartley, and my understanding from them is that it's better not to have a ground pour on top. The bottom layer is pretty much uninterrupted ground except two small traces and a section under the negative regulator (tied to the regulator body for some sort of heatsinking)

I added the jumpers to allow me to separate the circuits if I need to troubleshoot, they'll just be wire links in the final version

the board measures 65mm × 40mm

please feel free to tear it to shreds anyone, I can take it.

[MikeDB]

Well I always ground pour top and bottom. These things are massive EMI generators so you need to contain the shit as much as possible. There doesn't seem to be much ground underneath either. What are his reasons ?

On your layout, expose the copper under the regulators as well and a bit more on top. Left like this you'd be better off mounting them vertically.

[plushterry]

Well I always ground pour top and bottom. These things are massive EMI generators so you need to contain the shit as much as possible. There doesn't seem to be much ground underneath either. What are his reasons ?

On your layout, expose the copper under the regulators as well and a bit more on top. Left like this you'd be better off mounting them vertically.

My understanding of what he was saying is that for higher speed designs, having a ground pour on top only gives a small benefit (provided there is decent grounding on a layer immediately on either side) if it's done correctly and if not, it can make things a lot worse.

I was playing safe, basically. I have nearly solid ground across the whole back of the board.

Sorry, I had misunderstood about exposing copper, you mean no soldermask? Good idea, I'll do that. Thanks

[plushterry]

is this the sort of thing you mean?

[MikeDB]

Yes that's fine for heat.

He seems to have hours of videos and no quickly scannable literature, but I suspect what he meant was don't just ground-pour the PSU ground which is true - that can lead to circulating currents going everywhere. Instead I have a separate shield ground which is grounded away from the switching components, e.g by the regulator or power connectors, or even taken off the board on one of those mounting holes.

If you look at page 10 of the LTC3471 datasheet you can see this done well, with just the heatsink of the IC soldered to this ground, but totally enclosing everything else without joining to it. All those places marked GND on the upper side are connected together under the board. You could improve it further with careful point to point tracking, e.g. from D2 to C4, but a ground 'splodge' will do. Note the wire links they've use to pins 7 and 9 to avoid breaking this ground plane underneath.

Then connect this ground to all the others at the main grounding point, possibly the input power entry point to the PCB

[plushterry]

Nice one Mike, much appreciated.

I was trying to follow the example in the datasheet, but I couldn't get inductors with the same footprint as they had, so it got skewed a bit. I'd also assumed those wire links were traces on another layer! doh!


this was one of the videos I watched. It was the bit around 40:00 on copper pour I think (sorry wasnt Rick Hartley)

I found this one more interesting tbh. it is very long though,

[MikeDB]

Yes I use those inductors all the time as well. Here is a current layout I'm using them on. Not quite finished but you can see some key things like the one point of transfer to the ground plane using the vias by C37, single point of entry of the power by U5 (just realised this needs more vias !), and the surrounding ground plane. The outputs go to the regulators come from L1 vias and L3 direct. There's large capacitors near the regulators to smooth the supply before regulation. Some would argue these need to be nearer the switcher but I've tended to find placing them nearer the regulators works well for me.

The key thing with having single transfer points is it stops circulating currents getting into the main ground plane. Thus the current through the vias in and out should be just the changes in supply, which is already substantial, but not anything extra due to charge transfer between the Ls and Cs.

A simple test to see how well your completed design is, is to tune an AM radio to the IC switching frequency and probe around with a wire attached to the aerial to see where most radiation is coming from.

[plushterry]

That is really really helpful thanks!

so you're sort of funnelling all the grounds from the switcher together and sending them back to the main ground as one, rather than letting them scatter out and find their own way back.

I like the AM radio trick, will defo try that.