MAX1771 PSU instability
Jan Rychter
I'm looking for advice: I thought some of you here might have dealt with MAX1771 and know its quirks.
I've built a power supply based on Nick de Smith's excellent web page. I added a voltage doubler (for dekatrons), and a couple of linear stabilizers for other circuitry. I also built a larger current version (large inductor, RSENSE of 25mOhm). I tried to follow the PCB design advice very carefully.
I have a supply that kind of works, but I get a large sawtooth-like ripple on the output. The ripple is 17V peak-to-peak at 170V and the frequency is 23-80Hz (depending on the load). I'm loading the PSU with 25kOhms of resistance, which should pull 6.8mA -- so this is not an unloaded run. The ripple frequency seems to change with the load, the amplitude remains the same, though. Smaller loads seem to decrease ripple frequency, larger loads increase it.
I expected to see a ripple of 1-2%, but not 10%. Something seems to be wrong.
Any ideas or suggestions on where to look now?
--J.
John Rehwinkel
There are four things I would look at: current limiting, feedback oscillation, power supply problems, and thermal issues.
The MAX1771 has built-in current limiting, which could cause the whole shebang to cycle on and off, which could appear as a sawtooth after the output filtering. Make sure you have solid, low impedance connections to the current sense resistor and back to the CS input.
Power supply problems are the easiest - see if there's any similar oscillation at the power supply input pin. Nick's diagram shows separate power inputs for the inductor and the MAX1771 - are you powering them separately? Either way, look at the input power, if it's a lab supply that's going into current limit and retrying, you could get behaviour like this. If you're not powering them separately, it might be worth a try.
For feedback oscillation, you'd have a phase shift happening somewhere in the voltage regulation loop - or something that pretends to be phase shift. I'd look closely at the feedback resistors and make sure there aren't any parallel capacitors inadvertently hooked to them. I'd also carefully check the output capacitors - both the electrolytic and the high frequency one. If they're not doing their job of absorbing rapid spikes and hash, the controller chip can get confused about what's really going on. Scoping those points is tricky, due to all the high voltage, high current stuff going on nearby, which will tend to couple into the probe lead, upsetting the regulation further and confusing the scope display.
The last thing that occurs to me is a thermal issue. The MAX1771 will throttle down its on-time when it gets hot, which could lead to thermal cycling. You might need an external FET driver to switch your FET properly. Shottkey diodes get leaky when they're hot, but it doesn't seem to me that this would cause oscillation, I'd expected runaway instead. Your FET could change its characteristics when it gets warm, see if changing its heatsink changes the behaviour. And you could have a defective component that's just switching between working and not-working.
- John
Jan Rychter
On 13 sty 2012, at 17:17, John Rehwinkel wrote:
>> I have a supply that kind of works, but I get a large sawtooth-like ripple on the output. The ripple is 17V peak-to-peak at 170V and the frequency is 23-80Hz (depending on the load).
>
> There are four things I would look at: current limiting, feedback oscillation, power supply problems, and thermal issues.
>
> The MAX1771 has built-in current limiting, which could cause the whole shebang to cycle on and off, which could appear as a sawtooth after the output filtering. Make sure you have solid, low impedance connections to the current sense resistor and back to the CS input.
The board layout is right here, in case you'd care to take a look: https://skitch.com/jrychter/g2tq6/max1771-psu-1.0
This is heavily based on Nick de Smith's layout, although I might have made it worse. Of course I can share the full design if I manage to work out the bugs.
> Power supply problems are the easiest - see if there's any similar oscillation at the power supply input pin. Nick's diagram shows separate power inputs for the inductor and the MAX1771 - are you powering them separately? Either way, look at the input power, if it's a lab supply that's going into current limit and retrying, you could get behaviour like this. If you're not powering them separately, it might be worth a try.
Hmm. I'm powering the board from a (cheap) lab power supply integrated into my soldering station. It is supposedly capable of providing 1A @ 12V and I'm only drawing between 50mA and 200mA, but…
I looked at the supply with a scope and there are dips of around .75V that correspond to my ripple frequency. I thought those are to be expected. Nothing more serious, though. Would 1771 be that sensitive?
I have a single supply trace. There is a 100uF capacitor, then the inductor, and then the 10uF tantalum cap right next to the 1771. I never thought about separate traces for power.
> For feedback oscillation, you'd have a phase shift happening somewhere in the voltage regulation loop - or something that pretends to be phase shift. I'd look closely at the feedback resistors and make sure there aren't any parallel capacitors inadvertently hooked to them. I'd also carefully check the output capacitors - both the electrolytic and the high frequency one. If they're not doing their job of absorbing rapid spikes and hash, the controller chip can get confused about what's really going on. Scoping those points is tricky, due to all the high voltage, high current stuff going on nearby, which will tend to couple into the probe lead, upsetting the regulation further and confusing the scope display.
I thought feedback oscillation would result in higher frequency ripples. I don't see any parallel capacitors, just the ground plane below. My feedback path is substantially longer than in Nick's design, but it originates straight at the 4.7uF output reservoir capacitor and is relatively far away from anything else (everything around it is ground), so I thought I would be fine here.
The other modifications I made to the feedback path are: 1) I used two resistors in series because of high voltage and 2) my divider is really 1360k - 8k2 (+5k pot) instead of the more usual 1M5 - 10k (+5k pot), because of the resistors I had. I did not expect this to make a difference.
Oh, also, the final 100nF capacitor is not mounted yet (I don't have one). I assumed this would only make a difference for higher frequency switching noise.
> The last thing that occurs to me is a thermal issue. The MAX1771 will throttle down its on-time when it gets hot, which could lead to thermal cycling.
This is definitely not the case, nothing gets hot except for the load resistors, I haven't gotten anywhere near peak currents this should be capable of.
I will keep looking based on your suggestions.
--J.
marta_kson
that the feedback input is e x t r e a m l y sensitive to
interference. Try to decouple it to ground through a few hundred pF
and the problems might go away. I have not found the exact reason to
my own problems, but expect it's pulses injected to that input in some
way that changes the setpoint if the switcher is on or off. The data
sheet advices against a decoupling, but it seems to work.
Adam Jacobs
help wondering to myself exactly why anybody messes with these chips at all.
-Adam
Joseph Bento
On Jan 13, 5:16 pm, Adam Jacobs <a...@jacobs.us> wrote:
> I suppose that I only read about the bad experiences, but I always can't
> help wondering to myself exactly why anybody messes with these chips at all.
>
> -Adam
>
> On 1/13/2012 4:14 PM, marta_kson wrote:
These are very forgivable as to layout, and are even perfectly happy
built upon a piece of perfboard. Here's the article that everyone has
probably seen: http://www.ledsales.com.au/kits/nixie_supply.pdf
Joe, N6DGY
threeneurons
> help wondering to myself exactly why anybody messes with these chips at all.
efficient of all the switchers usually used here. Even the MC34063 has
stability issues, which I clean up in my circuit.
A system with feedback becomes unstable, if the loop phase hits 360
degrees before the loop gain drops below 1. There are two basic ways
to fix it. One is to thoroughly model the system, then add reactive
components to the network, to adjust the phase and gain to avoid the
above situation. The other is to swamp it, so that loop gain is
guaranteed to be below 1, by the time the phase shifts too much. I'm
lazy, so guess which method I use. Lazy method can't always be
applied.
Nick
with it is that my notes explicitly state that the FB trace should be
as short as possible, but in the layout shown it loops round the
board. See the "Key points" bullet list at
http://www.desmith.net/NMdS/Electronics/NixiePSU.html#design
You need to 'scope the FB pin - it should be very smooth - if you look
at my top mask, you'll see that the trace to pin 3 is very short -
http://www.desmith.net/NMdS/Electronics/NixiePSU/MAX%201771%20V5%20PCB%20top%20and%20bottom%20layers.png
Can you show us the schematic of your PSU? The arrangement of the
potential divider round the FB pin looks odd too, but its difficult to
be sure from just the board layout.
Nick
Nick
> I suppose that I only read about the bad experiences, but I always can't
> help wondering to myself exactly why anybody messes with these chips at all.
of this sort of switcher, so a bit more care and attention is
required, but the performance is unbeatable when you get it right.
Many folk want to step outside of the box - sometimes "just good
enough" is just not good enough!
Nick
marta_kson
The FB trace is definitely no good. It's imperative to keep it just as
a minimum pad right at the chip with just the two resistors connected.
Even just probing it with a scope might add enough stray capacitance
to pick up noise that makes it unstable. Also keep in mind that the
drain of the FET is an intense source of noise. My 2:nd attempt with a
single side board worked without decoupling after using a SMD to
ground and a ground trace all the way around the pad at this critical
pin.
Jan Rychter
> The PCB is very hard to follow with those dreadful colors, Eagle?
Yes, sorry about that. But Eagle is the only low cost (or free) option for hobbyists and it isn't bad for simple designs.
> The FB trace is definitely no good. It's imperative to keep it just as
> a minimum pad right at the chip with just the two resistors connected.
Hmm. To make the low voltage part of the FB trace any shorter, I'd need to get rid of the potentiometer. Otherwise it can't be made any shorter, the resistors can't be physically closer to the chip.
[time passes]
Well, after several experiments it turned out that after removing the pot and shorting it with a horizontally-laid piece of wire everything works just fine. So it seems that the pot (a Bourns 3296-style multi-turn potentiometer, about 1cm of height, as in http://www.bourns.com/pdfs/3296.pdf) was picking up interference. Could that be because of its vertical design?
But I'd like to better understand the comments (yours and Nick's) about the FB trace being too long. I thought that the critical part of that trace is the low-voltage part, from the resistor divider towards the FB pin. In my design the "long" part is actually just HV. I did not consider that to be very sensitive to EMI, as any voltage picked up here gets attenuated 20x or so by the resistor divider. Am I right?
The length of the HV trace to the resistor divider isn't different in my design and in Nick's design. It's just that I placed the output connector at the top of my board, while Nick has it on the bottom. But it's the same HV and it still needs to go around the whole chip and RSENSE resistor in particular. I could eliminate one row of vias next to RSENSE, which would make that trace 1mm shorter, but is it really worth the effort?
I think I'll need to redesign the board without the potentiometer, thus bringing the FB resistors much closer to the chip.
--J.
Jon
On Jan 14, 10:24 pm, Jan Rychter <jrych...@gmail.com> wrote:
> On 14 sty 2012, at 18:37, marta_kson wrote:
>
> I think I'll need to redesign the board without the potentiometer, thus bringing the FB resistors much closer to the chip.
>
used it. But if it's important to you to have an easily variable
output voltage and it's the pot which is killing you, then there is a
completely different strategy which works well. You can make very
satisfactory nixie and dekatron power supplies using microcontrollers
with on-board ADC and PWM modules.The PWM pin drives the switching
element in a standard boost SMPS circuit, and the HV feedback line
comes from a fixed potential divider into the ADC pin. You then
process the ADC output in firmware to determine the PWM duty cycle,
which gives you a continuously variable, programmable HV supply which
is great for playing around with things. Want to test the nixie at
160V or 200V? Just tell the microcontroller what you want the output
to be, and let the magic of negative feedback sort it out.
The downside is that it costs you some time overhead in the
microcontroller to keep the HV going, but with the right chip you can
do this, run a USB link and still have plenty of cycles left for a
funky user program. You probably don't get as good efficiency as
Nick's beautifully optimised 1771 circuit, but that is rarely a
terminal design issue in my experience. The efficiency drop has never
required me to heatsink the FET or anything like that.
I've run this strategy up to about 12W output - no doubt less than you
could get out of a thoroughly tweaked 1771 or John Taylor's awesome
modules - but plenty enough for most purposes.
Cheers,
Jon.
Jan Rychter
I develop software for a living, and I know how difficult it is to make reliable software. In the solution above I'd worry what would happen if my software went astray and the PWM controller happily continued to pump the voltage without any control whatsoever. I'd much rather use solutions which are self-balancing.
As for other suggested solutions (555 timers, etc) -- I learned already that a switching PSU is a complex beast, even though it might seem superficially simple. There are many corner cases that I'd rather have covered, such as: how does the circuit behave when the output gets shorted? When the short gets released? Is there overcurrent/overvoltage protection? Does it start reliably? Does it start when input voltage ramps up slowly? How does it react to sudden load changes? There are many things which one can get wrong, so I prefer an IC-based solution, where someone thought about all the corner cases.
--J.
Jan Rychter
My board was based on Nick de Smith's design. What I wanted, though, is higher current capability: I wanted to be able to draw 80mA and possibly more. I also wanted to have a second HV output through a voltage doubler (to get ~400V for dekatrons) and some additional stabilizers for digital circuitry.
I followed the advice given by Maxim in the datasheet and by Nick on his site -- reduced RSENSE to 0R025 (25mOhm) and used a large inductor (rated for 5A). The inductor is heavier than all the rest of the board combined :-) However, while the voltmeter happily indicated 180V at the output, the circuit was not stable: the MAX1771 was going into shutdown and there was a huge (30V) low-frequency ripple on the output. Ugly.
The advice I got from this group was that this was likely caused by noise on the feedback pin, and that my FB trace routing was no good.
Several board prototypes later (thank heavens for toner transfer, you can't beat the 30 minute turnaround time)...
As it turns out, the advice about the feedback trace was right, but only partly so. My problems were due to noise on the FB pin allright, but no amount of careful routing would have solved them. One way to get the circuit to behave in a stable way was to increase the current through the voltage divider. Even with 0805 resistors there is room to spare and going from 1.5MOhm total to about 300kOhm total meant that at least this part of the circuit was less susceptible to interference. However, I couldn't find a way to make the thing work with a (vertical) potentiometer and I don't think there is a way.
A 0R025 RSENSE resistor means that we're ramping the current up to 4A before releasing the energy stored in the inductor. 4A is a lot of current. The magnetic field produced by the inductor is so strong that it affects everything around it, even very carefully routed traces. A scope probe held in the air near the pot picks up almost .6V of interference! This only goes up as one approaches the inductor. Depending on how the inductor is mounted (which side of the board) you can get voltage increases or voltage drops on your FB pin.
I did some experimenting and:
-- moving the inductor away is a solution, but it needs to be *far* away, 8cm or so,
-- shielding the inductor, while improving the situation, increases the current consumption 2x, produces audible noise and heats up the shield considerably, so it is not a solution.
All in all, I don't think a circuit with an RSENSE of 0R025 is feasible, at least not with a 5cm x 5cm board. I'll be going back to 0R050 and 0R100 and smaller inductors.
I can post some scope traces if people are interested. I have learned a lot in the process, and as a nice side effect I have a pretty clean PCB layout that is realizable with a single-sided board (requires one jumper) -- this might be useful for people who make their own PCBs. Once I get it verified and tested I plan to post it for people to use.
--J.
John Rehwinkel
> I did some experimenting and:
>
> -- moving the inductor away is a solution, but it needs to be *far* away, 8cm or so,
>
> -- shielding the inductor, while improving the situation, increases the current consumption 2x, produces audible noise and heats up the shield considerably, so it is not a solution.
>
> All in all, I don't think a circuit with an RSENSE of 0R025 is feasible, at least not with a 5cm x 5cm board. I'll be going back to 0R050 and 0R100 and smaller inductors.
Have you tried a toroidal inductor? They're better behaved in this respect, even though they're physically large, especially for the high current one you'd need.
Here's a datasheet from one manufacturer:
- John
Jan Rychter
>> A 0R025 RSENSE resistor means that we're ramping the current up to 4A before releasing the energy stored in the inductor. 4A is a lot of current. The magnetic field produced by the inductor is so strong that it affects everything around it, even very carefully routed traces
>
>> I did some experimenting and:
>>
>> -- moving the inductor away is a solution, but it needs to be *far* away, 8cm or so,
>>
>> -- shielding the inductor, while improving the situation, increases the current consumption 2x, produces audible noise and heats up the shield considerably, so it is not a solution.
>>
>> All in all, I don't think a circuit with an RSENSE of 0R025 is feasible, at least not with a 5cm x 5cm board. I'll be going back to 0R050 and 0R100 and smaller inductors.
>
> Have you tried a toroidal inductor? They're better behaved in this respect, even though they're physically large, especially for the high current one you'd need.
Hmm, I haven't considered that. They might indeed behave better. The inductor I use is from a Polish manufacturer: http://www.feryster.pl/polski/dsz14x15v.php (except I used a 5A version).
But overall I think I'll try the smaller RSENSE values first, they should be enough to provide the output currents I need.
--J.
Charles MacDonald
>> Have you tried a toroidal inductor? They're better behaved in this respect, even though they're physically large, especially for the high current one you'd need.
>
> Hmm, I haven't considered that. They might indeed behave better. The inductor I use is from a Polish manufacturer: http://www.feryster.pl/polski/dsz14x15v.php (except I used a 5A version).
>
That site has "Energy storage and interference suppressing chokes in
SMPS power supplies, wound on RTMSS type toroidal cores"
http://www.feryster.pl/polski/dtmss.php?lang=en
--
Charles MacDonald Stittsville Ontario
cm...@zeusprune.ca Just Beyond the Fringe
http://users.trytel.com/~cmacd/tubes.html
No Microsoft Products were used in sending this e-mail.
misty01a
In my "high current" MAX1771 PSU design I made several years ago, the
best results I got when I used a toroidal inductor with a current
rating of 10.3 A (Bourns 2200LL-470-RC), and a RSENSE peak current
setting of 5.33 A. I tried other inductors, including a physically
smaller 2100LL series inductor (with a smaller current limit), but the
efficiency was not good as the 2200LL. I don't know why.
Several notes that may help (based on my personal experience only):
- The FET drain tab is the source of a great amount of noise. The FET
drain should be placed as far away from the FB pin trace as reasonably
possible. An SMD (D2PAK) FET may be better than a TO-220 one because
of the horizontal placement on the PCB (also for better cooling of the
FET).
- I have never observed any interference from the inductor, but then I
use toroidal inductors which are supposed to be self-shielding. I
once did get good results with an unshielded Bourns 1110 series
inductor, however.
- For RSENSE I use several 0.075 Ohm 1/4 W resistors in parallel.
They are cheaper than a single larger resistor, and it's easier to
adjust the peak current value.
- A diode between the REF and FB pins may help if the MAX1771 has
trouble starting up. The MAX1771 can enter 12 V fixed output mode if
the supply voltage is larger than 12 volts and the voltage at the FB
pin is too low (because of the high input:output ratio of the voltage
divider). On the other hand, many other people's designs seem to be
working fine without this diode.
My present design uses a Bourns 2200LL-470-V-RC inductor and an
FDB28N30TM FET (0.129 Ohm ON resistance). The maximum power output in
a testbench situation was 24.9 W at 85 % efficiency with 14 V input
and 220 V output. Board size is 50 mm x 40 mm. I use three of these
units in parallel to provide 40 watts at 250 V in a (non-Nixie)
project.
Jan Rychter
I have one more question -- did you use a potentiometer in any of your designs? This *really* makes a huge difference in my tests.
As for the drain being the source of noise -- right, this is the pulsed inductor output, with monstrous voltage peaks and high currents. But there is a limit to how small one can make it and how far away from the feedback network it can be. You might be right about an SMD FET being better here, though.
Great tip about several resistors in parallel for RSENSE, too :-)
thanks,
--J.
> --
> You received this message because you are subscribed to the Google Groups "neonixie-l" group.
> To post to this group, send an email to neoni...@googlegroups.com.
> To unsubscribe from this group, send email to neonixie-l+...@googlegroups.com.
> For more options, visit this group at http://groups.google.com/group/neonixie-l?hl=en-GB.
>
misty01a
reason is, they make it more difficult to do a better PCB layout, and
anyway the regulated output voltage from the supply using fixed 1 %
resistors is accurate enough for the purpose of powering a Nixie
display. I could always replace the resistors with different values
if I wanted a different output voltage.
I wish you good luck with the TPS40210 design.
By the way, I do use trimpots in the microcontroller-based supplies
that power my more recent Nixie designs. This is because I use a
built-in comparator instead of an ADC, and the reference voltage is
not specified as precisely as a purpose-built controller. I'm
probably as concerned as you are about the reliability of the
controlling software. Safety can be improved somewhat by placing a
high-pass filter between the uC and FET driver, and also making the
software create a series of one-shot pulses instead of letting the PWM
controller run freely.
Ken