SEPIC pre-regulator for µSupply clone? Opamp supply? [sorry, long]

[0xdeadbeef]

I was fascinated by the µSupply project from the beginning but I waited for so long now and it went into a direction that I don't fully like, so I toyed with the idea of building my own small mini supply.

I will replace the LT3080 with a LT3081, remove all the battery stuff, drop the USB power supply option and use just one DC supply. As a side note: I would have loved to use only the USB supply, but the measly 600mA from an USB2 would have limited the current capability too much, especially when using an isolated DC/DC with a typical efficiency <80%.

So in a nutshell I want to use something like a 5V/2.5A (or 3A) power supply which is cheaply available for USB ports and stuff like that and create an output up to 15V at 500mA (1A for <=5V or so). Another option would be a 9V supply. We'll come to this later.

Now I could use a step-up converter as the µSupply does, but then the voltage drop on the LT3081 would be relatively high for smaller voltages resulting in higher losses and temperature. E.g. when creating 1V at 1A (intentionally or in current regulation), instead of wasting 1.5W-2W at the LDO (1.5V worst case voltage drop + shunt), the losses at the LDO would be up to 4W. So I thought about using a step-up converter in a SEPIC (single ended primary inductance converter) configuration where it's possible to adjust the regulator output not only up to 17V or so, but also down to like 2V. The SEPIC configuration is not the most efficient one, but I like the idea to not burn power/energy at the LDO - mainly for thermal reasons.
I first thought about using a LM2577 as in the Chinese SEPIC converters sold on eBay, but it has a switch frequency of only 52kHz, so I investigated a little further, thought about a LT1170 (100kHz) and finally decided to use a LT1370 (500kHz). One of the benefits of using another LT part is obviously that I can simulate the circuit including the LT1370 and LT3081 in LTSpice.

However, lowering the regulator voltage creates some new issues. Since most high side current monitors like the ZXCT1009 or INA139 use the common mode voltage also as supply voltage, they would force me to create a regulator voltage of at least 2.5V (INA139: 2.7V) while the regulator voltage needs to be only ~2V above the output voltage (1.5V for the LT3081 + 330mV for the shunt + some safety margin). This would mean another half Watt wasted at 1A.
So I dropped the ZXCT1009 for a LT6105, mainly since it has a supply voltage independent of the common mode voltage. Well, and the availability is much better. Any hey, another LT part I can simulate.

Finally, I replaced the LM324 with the precision substitute LT1013. This decision is discussible since the price increase is probably much higher than the increased benefit, but for the moment I like the idea of lower offset voltage and having another LT part to simulate in LTSpice. However, the regulator output going down to e.g. 2V also affects the Opamp supply. The minimum supply voltage for the LT1013 is 3.4V (LM324: 3V), so I need another supply for pre-regulator voltages below that. I decided to use two diodes to use either the 5V supply or the pre-regulator output. This works despite of quite some ripple on the Opamp supply in current regulation scenarios which is probably not the perfect base of stability.

So the circuit works in principle (in LTSpice), but feeding the Opamps from the pre-regulator output still seems like a hack. The problem is that it limits the rising of the "set" voltage quite considerably. It takes like forever to raise the voltage from 0 to 15V because when you start at 0V, the preregulator voltage is e.g. 2V and so Vset can reach only 1.8V or so. Only when the pre-regulator voltage increases a bit, Vset at the LT3081 increases and the output voltages slowly rises. Besides the very slow gradient, there are also stability issues. I guess this is because any underswing on the pre-regulator voltage during a rising voltage also lowers Vset which creates an ugly oscillation.

Anyway, all the problems are cured when I provide the Opamp responsible for Vset with a stable 18V supply. Now the problem is how to create this voltage with a 5V DC supply. Using a 2nd DC/DC sounds like overkill. Maybe it would be possible to cascade two voltage doublers like ILC7660 (20mA) oder better MAX660 (100mA) to reach 20V, but this looks like a workaround as well.
The only other (more or less) simple option I can think of is to use a 9V DC supply as input for the SEPIC converter and create 18V from it with a charge pump (e.g. MAX660).

Any other ideas?

BTW: attached is my current LTSPice model. Some parts taken from the last USB uSupply design, some replaced. The microcontroller part (on-chip DAC for current setting, PWM for voltage setting, ADCs for I,U,Temp, display etc.) is missing. Values are not optimized and I didn't test excessively, but it looks somewhat promising. Constructive comments on the circuit so far?

[hugo]

Have you seen this "High Performance Portable DC Bench Power Supply" :
 
http://www.linear.com/docs/45095

[0xdeadbeef]

Sure, but it uses current regulation based on the ILIM feature of the LT3081 which not very exact. For the moment I decided to ignore it and use the current regulation from the uSupply design.
It also uses a stepdown from a high input voltage and sets the voltage and current through pots. in the end, I could not use anything from that design.

Anyway, I'm facing some issues with the current regulation which leads to ugly sawtooth oscillations on the current for small loads. For the moment I can only lower their amplitude if I decrease the overall regulation speed. I'm not really happy with this and have to investigate if I find a better solution.

[0xdeadbeef]

Ok, some things learned during the last day of messing around:

1) The ESR of the output capacitor is really important. With 0.08Ohm I had weird oscillations at higher voltages, with 0.04Ohm they are gone.
Since it will be hard to find a 220µF capacitor with 0.04Ohm, I will probably use two 100µF caps with 0.08Ohm ESR in parallel.

2) Any oscillation on the DCDC converter's FB pin tends to propagate to the regulator output.
Putting a 1nF capacitor from feedback pin to ground improves the behavior dramatically.

3) The sawtooth oscillation in the current regulation was caused by the LT1013 being pretty bad as comparator.
Don't know if the main cause is propagation delay or saturation or both, but replacing it with a comparator (e.g. LT1011) decreases amplitude and magnitude of this oscillation to something I can live with.
I wonder if the LM324 is much better in this regard, if some other difference in Dave's design compensates this or if the same issue exists in the uSupply design.

My original problem remains anyway: how to create the 18V for the Opamp supply?
I realized now that the MAX660 will only accept supply voltages up to 5.5V or so and the ICL7660 is marked as obsolete. This more or less leaves the ICL7662 as only choice.
Or I could build my own charge pump with a µC PWM...

[prasimix]

My original problem remains anyway: how to create the 18V for the Opamp supply?

If you want to skip µC PWM charge pump or one based on LM555 here is one interesting alternative. This could be possibly better source for driving charge pump since in your case you need voltage quadrupler not just doubler. Please note that suggested article do not address quadrupler circuit, that you can find on many other sites.

P.S. Maybe some members here would like to have also model in .asc instead of .png format

[0xdeadbeef]

Indeed I played around with a dickson charge pump later today. From my LTSpice experiments it looks like I could create ~20V from a 5V supply. So I can probably keep the 5V supply idea.
Under a 1mA load it goes down to 17.5V, but this should be still sufficient for the one OpAmp I guess. Problem is that my µC is a 3.3V type and has only one high current output anyway.
So to boost up a 5V voltage, I need two external MOSFET push-pull-stages (two half bridges).
Unfortunately, PNP push-pull-stages won't work as the voltage drop on the junctions adds up with each stage and I'm a bit scared to use a discrete FET-halfbridge (latch up).
For a simulation I used a LTC1693-2, which works perfectly (especially since it has an inverting and not-inverting input) but is much too expensive. I had no luck yet though to find something cheaper yet.

Anyway, I attached a zip with my current models. Note that they are not perfect. It's just something I use to play around.

[EDIT]
The Microchip TC4428 looks promising as driver for the charge pump. It's relatively cheap, easily available and has an inverting and non-inverting output. I downloaded a spice model and will try to get it to run in LTSpice tomorrow. Need to get some sleep now

[0xdeadbeef]

Hm, this is getting a bit frustrating. The models for TC4426/TC4427 (as replacement for TC4428) were generating simulation faults and when I got them running, the simulation was painfully slow. Even worse, the TC4426/7/8 behaves like a BJT push pull stage even though the manual depicts a CMOS stage. I wanted to try the beefier TC4425 but the according models for TC4423/TC4424 are not working at all. No output generated whatsoever. Then I wanted to try a LM5111-3M but learned that Spice models from TI are encrypted and can't be used with LTSpice.
IXDF602 or IXDF604 could be an option, but there is no spice model for them.

[EDIT]
I kinda underestimated the influence of the switch resistance.
[...Removed partly wrong conclusions to avoid confusion...]
Problem is that for 10mA flowing at 20V, there's at least 40mA flowing into the circuit at 5V. Which means a voltage drop of e.g. 0.4V for 10Ohm switch resistor. For three pump stages, this sums to 1.2V plus the 0.3V (BAT54 at 1mA) per diode for 4 diodes means a drop of 2.4V or 17.6V instead of 20V. Which means that to get 10mA out of the charge pump at a voltage > 17V the switch resistance should not be bigger than 10Ohm at 5V.

[0xdeadbeef]

To continue my monologue, I redesigned the dickson charge pump so it works with 10nF caps and a TC4425A. This is still a 1.5€-2€ part in small amounts, but I was unable to find something much cheaper with comparable specs and good availability.
While the manual specifies the in/out resistance as 2.5Ohm typically at 18V, my (simulated) measurement hint towards something around 10Ohm at 5V.
To estimate a fitting switching frequency, I used a 2*tau approach (as 2*tau is the time where a capacitor is loaded by 86.5%).

2*tau = 2*R*C = 2*10Ohm*100nF = 0.2e-6 = 2µs -> 500kHz

With these numbers (TC4425A with ~10Ohm switch resistance at 5V, 100nF caps in the pump stages, 500kHz frequency) I can draw at least 12mA while the output voltage is still > 17V.
Note that even with an efficiency of 100%, a 12mA draw at 17V means 40.8mA (17/5*Iout) mean current flowing into the input.
For 41mA, the voltage drop due to the switch resistance is about 0.41V per pump stage or 1.23V in sum. When adding around 0.3V drop per diode, this is another 1.2V drop.

20V-(0.41V*3)-0.3V*4 = 17.57V

Note that I used 17V/5V to calculate the output current which is a bit of a cheat. Still the estimation is a bit better than what I measure (~17.1V at 12mA), so I guess it's good enough to show the influence of the switch resistance.
So when using a cheaper option like the TC4428A with a much higher switch resistance, the voltage drop will be higher which means less current can be drawn. It's not like I really need >10mA but for the moment I like the idea to have a bit more current available than I need. I can still replace the TC4425A with a TC4428A later since they have the same pinout.

[0xdeadbeef]

And another update to my monologue.

Firstly, I kinda decided to change the DC input to 9V. Total efficiency at 15V out is much better (about 83% instead of 75%), also the input current needed is generally lower.
Indeed, 15V/1A would be theoretically possible now.

With 9V the charge pump is reduced to 1 stage and I can use a single driver like a MCP1406/07. Not much cheaper than a TC4425, but the whole charge pump will take less space.
Main drawback is I'll need a 5V linear regulator but on the other hand, this solves the problem for strict overvoltage protection on the DC input. Probably, I'll use a PFET as reverse protection and that's it.

I also started playing around with using Imon instead of an external current measurement. At least in the simulation, the results look great. The current regulations works much better and this would not only save the shunt and the LT6105 but I could also lower the offset and thus increase the efficiency. Well, at least in theory.
My main issue with this is the unknown accuracy of the Imon output. Apart from a min/max rating, the datasheet gives no information whatsoever, just an ideal diagram without temperature/voltage influence and no absolute error values or whatever.

[prasimix]

I also started playing around with using Imon instead of an external current measurement. At least in the simulation, the results look great. The current regulations works much better and this would not only save the shunt and the LT6105 but I could also lower the offset and thus increase the efficiency. Well, at least in theory.
My main issue with this is the unknown accuracy of the Imon output. Apart from a min/max rating, the datasheet gives no information whatsoever, just an ideal diagram without temperature/voltage influence and no absolute error values or whatever.

Maybe you can contact Frex on diyaudio forum. He is using Imod output in his solution. Here are schematics.

[0xdeadbeef]

Maybe I overlooked something, but it seems like he is using the Imon output just to measure the current via an SPI ADC. It doesn't seem to be involved in the current limitation which again seems to be done via the ILIM feature (through current mirror). My understanding is though that the internal current limitation is not very accurate (+/-15% over temperature) which means I would expect a current regulation in the 10mA range while I aim for the 1mA range. Problem is that the Imon accuracy is not specified. If it's too more in the 10% range than in the 1% range, I guess I need to go back to the external current measurement.

One thing I spotted in this schematics and which I had already added to my model in the meantime is a clamping diode from Vset to the output. This is because the manual warns that the internal clamping diodes are build to handle only up to +/-10V but e.g. a hard short circuit on the output while Vset is still 15V could possibly damage the device.
Also the other direction is critical: switching Vset to GND while the output is > 10V. This will usually only happen when switching OFF, also my output capacitor is low and I have a 5mA current source in the output. Yet it's worth thinking about a soft shutdown and limiting gradients to avoid Vset being much lower than Vout.

One last thought: I noticed only now fully that the LT3080 used in Dave's design uses separate IN and VControl pin where the manual says
"The current flow into this pin is about 1.7% of the output current"
Which means 17mA at 1A. The current measured is however only the one going into the IN pin. Which looks correct at first sight, but the current through the load is Iin + Icontrol - Iset (where Iset is fixed to 10µA and thus can be ignored). So when the current measured at the shunt is 1A, the current going through the load is 17mA higher.
The LT3081 is different in that it has only one common supply/input pin.

[prasimix]

Maybe I overlooked something, but it seems like he is using the Imon output just to measure the current via an SPI ADC. It doesn't seem to be involved in the current limitation which again seems to be done via the ILIM feature (through current mirror).

You understand it correctly. Imon goes to ADC and Ilim is controlled with DAC (via current mirror). He made in that way a CC control loop if I understand correctly. How accurate that could be I don't know.

[0xdeadbeef]

I wouldn't call that a current control loop. The actual current limitation is only in the LT3081. Someone here in the forum claimed a while back that the ILIM feature would just turn the current off and not try to keep the set current. Honestly from the manual I can't tell whether this is true or not. I guess I will setup a test to investigate this. Nevertheless, I don't think that I will use the ILIM feature anyway.

Side note: the 1µF I currently use at the SET pin is fine for resistive loads, but for capacitive loads, I'm ending up with sawtooth current/voltage at the output. So I will probably have to increase the value, I'm just not sure yet to what value or better: what kind of design approach to use to select a sensible value.

[EDIT]
Well, I played a bit with the ILIM feature.
I removed the current control from my model and added a 1839Ohm resistor between OUT and Ilim to set the limitation to 500mA.
0.5A/360mA*1000Ohm+450Ohm -> 1838.88Ohm

Well, with a 15Ohm load and SET=15V this results in a 577mA current through the load which is 77mA (!) too high.
With the clamping diode between SET and OUT this current is even higher since the output is ~8.65V while the SET voltage is 15V.
In a short circuit situation (0.2Ohm load), the current through the load is even 581mA. Again, this would increase with the clamping diode.
Note that 81mA error at 500mA off is not even in the tolerance of +/-15%. So while Ilim really provides a perfectly well implemented
current limitation, which is very fast and stable, the absolute accuracy according to the LTSpice simulation is very bad and even outside
the claimed +/-15% accuracy. Maybe this could be partly overcome by calibration, but as there's also a temperature dependency, I'd currently
assume that the Ilim feature is not usable for a fine current limitation in a lab power supply.