Another Power Supply

[mij59]

As a bonus, the two MOSFETS will naturally equalise current so I'm not as worried about one getting hotter than the other (like I was before). I should mention as well that the NTP5864N is good to 175 deg
For bonus points as well - the data sheet specifies a max Rds of 12.4 mohm. With a 100 mohm pass resistor, then at 2A I could expect a ~225mV voltage drop, which means I can (maybe) regulate to 24V! 

Equalising properties only apply when the mosfets is used as a switch, when used in a linear power supply the mosfets are  used in the linear mode.
At a junction temperature of 175 C the maximum drain current is zero.
The maximum Rds is not important the mosfet is not used as a switch.

[SteveP]

[Others chimed in before I finished typing....but here it is anyway...]

You seem to be having fun! Glad to see you've wriggled out of the grasp of the heat demons (at least temporarily). Here are a few comments:

1) When you start cutting things a bit close, you need to take into account things like the fact that mains voltage isn't always on spec; sometimes it's less, sometimes it's more. Your 18VAC may be a bit higher making your drop a bit larger. I used 10% in my calcs, just to be safe. Even 5% gives you a 26.8v drop * 2.5 A = 67Watts / 2 = 33.5 W * 4C/W = 134C + 30C = 164C/175C = 92% of spec. That's far too close for my comfort. There's a general rule of thumb that says for every 10C drop, you double the lifetime of the component. The mfrs don't spec *lifetime* at Tjmax, so you're kinda guessing on that one. But as I indicated before, I try to run my devices fairly cool.

2) You're talking about running mosfets in parallel. It *can* be done, but you're wandering into a bit of a snake-pit. Just from the point of view of heat (that is, leaving aside the issue of controlling them in a feedback loop), the problem is that below a certain threshold they *don't* share current equally (I had forgotten this until Kleinstein mentioned switching vs. linear mode back a few replies). The explanation can be found here:

http://www.infineon.com/dgdl/Infineon--AN-vNA-NA.pdf?fileId=db3a30433e30e4bf013e3646e9381200
(if the link doesn't work, go to Infineon's website and search for "AP99007")

Still, HP ran 4 IRF440 in the 3610 with no resistors (that I could find in the schematic), so maybe with enough derating it isn't as hard as it seems.
Edit: oops, found them. 10 ohms, but only one resistor per *pair* of FETs.

Anyway, let's do a heat calc in reverse, assuming a max jct temp of 175C and assuming you don't run it at more than 150C (86% of max--still pretty high...):

150C -30C (ambient) = 120C / 70W (round numbers) = 1.7 Rtheta (total) C/W - .5 C/W (Rtheta device) = 1.2 C/W Rtheta heatsink. I did a quick digikey search (US) and about the cheapest I could find was $15.

So now you need to find an n-fet that:
1) Has a Tjmax of at least 175C
2) Handles 300W (which is an indirect way of finding one with an Rtheta of 0.5C/W)
3) Doesn't have much more than about 3000pF of input capacitance (more on that later)
4) Has a SPICE model you can get your hands on

(4) is tough...and you definitely want to be able to sim them. I did a quick search and didn't quickly find one that I could find a spice model for. The 175C reduces your selection by quite a bit, but that's kind of forced on you because of your volts*amps decision.

Without trying to push you in a particular direction, I did the following calc:

150C Tjmax running at 125C (83%) - 30C (ambient) = 95C / 1.7C/W total Rtheta = 56W  = 25V * 2.24 Amps. That's not much of a reduction in your volts/amps envelope.

Or....you could use a CPU cooler (with a fan) ....really good Rtheta and small ones are cheaper than big heat sinks....

=================
Now about that input capacitance...

I won't try to go into chapter and verse here, but mosfets have capacitance built into them, some more than others. Very roughly speaking, the bigger the die, the more the capacitance. OK, pick one with a small die, right? You'd like to, but heat dissipation (Rtheta) is proportional to die size! So, if you want to be able to handle a lot of power, you end up with a bigger die which means more capacitance.

So what's the big deal with capacitance? One way to look at it is that it slows down the response of your feedback loop. A slow feedback loop means that things get out of whack for a longer time (thereby being more out of whack) before the control mechanism can catch up and correct the situation. It also makes it harder to create a compensation network for the opamp because it creates a low-frequency pole (or moves an existing one further down in frequency). Finally, if your PSU has (or will have) a "mute" or output enable/disable switch, then you can get a big spike at turn-on if the fet has a lot of capacitance.

If capacitance weren't an issue, you could just go for a super-low Rtheta and be done with it. Sadly, it is an issue.

--Steve

[braddrew0]

Steve why 2.5A? I was only using 2.5A for my ripple calculations because I had 2A through the pass device but 500mA set aside for he uC, display, etc... which shouldn't go through the pass device?

OK, one more try... what about MJ11028 (http://www.onsemi.com/pub_link/Collateral/MJ11028-D.PDF) which has a theta jc of 0.58 and this heatsink from Wakefield Vette (http://www.digikey.com/product-detail/en/423K/345-1050-ND/340346) with a thermal resistance of 0.96 non-forced? That's a total of 1.54 deg/W, so at 68W it's a rise of approx 105deg... the darlington is good to 200c, so even adding ambient (and say a 10-20% load increase) I'd still be well below the max?

[braddrew0]

OK working on the assumption of a single MJ11028 I spent a few hours this morning running simulations. The first thing I noticed was that it seems "slower" than the last device which kind of makes sense - I'd imagine a 300W TO-3 would have more capacitance than a 70W DPAK but this information doesn't seem to be in the datasheets? The integrating cap of 1uF only gave 5 degrees of phase margin and there was noticeable (about 20mV) of ripple on a simple 100 ohm load.

I've played around with this, but also the big thing I worked on was output impedance. The original circuit gave about 38 ohms at around 60Hz - which is a fair cry from 5 ohms at 50kHz (which is the easier end of the range you gave me Kleinstein). I changed the value of a lot of components, but the best compromise I could come up with was 10.7 ohms at 160Hz. I could get lower by changing the resistor divider, but it required significant capacitance on the integrator (5uF+) which gave an unacceptable time to decrease voltage (20V-0V took > 5s). I could also move the peak to a higher impedance by changing the output cap, but this gave extremely sharp peaks, and started introducing multiple peaks rather than the "smooth" curve I ended up with. Best case, I still couldn't get it much higher than 1kHz, and that gave me a completely messed up looking response. Again, I'm putting this down to a "slow" pass device.

So here's what I ended up with, and a few results.



This is the circuit - please note the picture looks like an NPN but the model is a darlington (had a few issues with getting it to display the correct picture). The output cap is based on a real device (panasonic low ESR 100uF cap) and I've added in the current sense resistor.



This is the transfer function. I spent a bit of time trying to smooth out that second peak, and it looks reasonable to me. There's about 25 degrees of phase margin here - I found if I dropped the cap much lower, it would raise the peak on the right which would give me two 0dB values - the worst one being completely unstable (220+ degree phase shift).



This is the output impedance. Like I said before, it's about 10.7 ohms at 160Hz. Phase is between +/- 90 deg across the range so should be stable for all loads.



This is driving a low ESR cap (1uF, 0.001ohm). It doesn't take too long to reach max voltage and it's rock solid once it gets there.



For stamps, I looked at 0V output. Much better than last time, which I assume is from the resistor on the output of the opamp.




This is a step input from 0V to 20V. As expected, it's very similar to the low ESR case.



This is a step input from 20V to 0V. This is the one that would blow out with higher values of capacitance on the opamp. This is much more stable.



And lastly, this is a pulsed load. I went 1mA up to 2A, switching every 10ms. That's a maximum of about 20mV over/undershoot.


So that's where I'm at now. For my purposes, unless there's something I've overlooked, I'm pretty happy with where it is here. I get that it's probably not the "best" possible design, but it's stable, it'll do what I want it to (I think) and most importantly it won't explode.... I think

So next step is adding the current limit right?

[Kleinstein]

The large transistor might be relatively slow (can't see anything in datasheet).  It's also a quite large one - two smaller ones (e.g. TIP3055 or similar - still not fast) could be cheaper and more choice. Having a small resistor at the emitter also often helps to improve stability - so the resistors needed for current sharing are also helpful.

The resistor from the OP to the transistor is rather large - this could be a problem with such a large transistor.

To protect the transistor from excessive negative base-emitter voltage, a diode from base to emitter can help.

Normally one would have the divider higher impedance, by a factor of 10-100. This would also bring the integrating capacitor to the more normal range.

One can also improve phase margin by adding a RC series combination in parallel to R3. Though normally this is not needed with this type of regulator.

[blackdog]

Hi braddrew0,

You must be kidding...
And R6 = 1K
R3 720 Ohm, R4 180 Ohm.
C2 = 1,2uF     


The OpAmp   
Max 1.2mA output current.

You've done almost everything wrong, how is this posible.

OK, now the help
We start with R3 and R4, make them 10x the value.
C2 = 330pF to start with.
The opamp, try LT1007
R6 = 150 Ohm

Also place a capacitor of 100uF between the collector and R2.

Play with C2 and the capacitor on the output C1, C1 average value = 50uF/Ampere output current.
If you need far more for a stable designs, than adjust C2 to 470 a 560pF.

You need about 1mA current from the opamp output for 2-Ampere output to de load.
I do not know how much current you need and how much dissipation, but several TIP142 transistors is normaly a better solution.
Each with its own base and emitter resistor.

I hope tho see results from you, and think about your circuit, wy the value's are wrong, you will learn a lot of it :-)

Kind regarts,
Blackdog

[braddrew0]

Thanks Kleinstein - what range is "small" for the emitter transistor? I'll start at 1 ohm and see what the results are like. As for the BE protection diode, I hadn't seen that one before, so thanks - I'll add something in. I had the divider at 4k/1k but lowered it to try and drop the output impedance. Good tip on the extra RC network- I'll keep that one in my back pocket for the next design. And I'll put something together with parallel BJTs today. Thanks again

Hi blackdog - thanks for the input! Nope, I'm not kidding, I'm just trying to learn As to how I ended up where I ended up, it can be pretty much summed up as:

* The pass device was the only one I could find that would drop 68W without spending $150+ on a heatsink
* As you say, I planned on 1mA of current for 2A so I didn't see the 1.2mA max current of the opamp as a limitation
* I started with 4K/1K as the divider, but this gave me about 38ohm output impedance - I dropped them down progressively until I hit the values on that schematic, which gave me closer to 11ohm
* Lowering R6 made the "peak" of the impedance graph much sharper - I started with 120 ohm, but progressively increased to 1k to "smooth" out the impedance graph. Again, because max current through was only 10mA, I didn't think this would be much of an issue
* Based on R6=1K, any lower than about 1.1uF made the circuit unstable with noticeable ripple in the output. I took 1.2uF as the next standard value

And that's what got me where I am I'm going to rework the design this afternoon and I'll try out the suggestions you made - thanks for your help, I appreciate it

[braddrew0]

OK, simulations run! Here's the new circuit:



Changes are:

* Four TIP142s - these have a low theta jc (1.0 deg/W) and with cooling, they'll each dissipate about 3.7 deg/W (to a max of 150C). Three will technically be within limits (about 85 rise each) but four gives a little extra room (63 rise each). This means that if one starts passing more than another, I've got a bigger buffer until they hit the limit

* Added 1 ohm to each of the emitters for stabilisation

* Each TIP142 now has a emitter-base protection diode (MBRS360T3 - 60V/3A schottky)

* Increased feedback network to 20K/5K (approx 25x increase)

* I looked at the LT1007 but unfortunately it's not rail to rail so will struggle on my single supply design. The LT1677 is a higher current version of what I had - compared to the LT1007 is about 4 times slower with about 10-20% more noise. LT1007 will definitely be first pick for the next design!

* blackdog - I'm unsure what you mean about a cap between R2 and the collector... won't this just block the DC going through?


So with all of this in, I played around with the value of C2. Starting at 330pF, I found a phase margin of 1.4 degrees. There was noticeable over swing on the output, but it was definitely fast! My only question is on the stability of that circuit - AN-1889 (http://www.ti.com/lit/an/snva364a/snva364a.pdf) and everyone's favorite Wikipedia (https://en.wikipedia.org/wiki/Phase_margin) both state a minimum of 45 degrees of phase margin is required for stability. AN-1148 (http://www.ti.com/lit/an/snva020b/snva020b.pdf) from Steve before says to aim for 20 degrees.

With that in mind, I increased C2 using standard values until I got a phase margin of first 20deg then 45deg. I hit 20deg at.... 1.2uF 45deg required 3.3uF. So I guess my question is... do I really need that much phase margin? I ran a bunch of simulations (I'll stick below) and ignoring bode plots and impedance and whatnot, the actual output looked useful to me. So do I really need 20deg, or is 1.4 good enough?

Here's the plots:



330pF transfer function




1.2uF transfer function




3.3uF transfer function




330pF impedance




1.2uF impedance




3.3uF impedance




330pF under a switching load (1mA to 2A every 1ms)




1.2uF under a switching load




3.3uF under a switching load




330pF pulse input (0V-20V-0V output selected)




close up of the overshoot on the 330pF pulse input




1.2uF pulse input


I couldn't do a 3.3uF rise-fall chart because it was too slow to hit the right output values in time    Not shown is the 330pF on startup hits about 21V before pulling back to 20V...
I've also added my SPICE files if they're useful.

Thanks again guys, appreciate all the help

[Kleinstein]

The diodes used for protection do not need to be so large, they just have to prevent the OP going much more negative than the output. So just a single 1N4148 is good enough. Its also better to go directly to the OP - this helps a little with recovery from saturation.

The phase margin depends very much on the load capacitance. With just a low ESR cap and current sink  at the output the phase margin will be about as low as it can get. For this case a small margin of 20 degree or even slightly less is OK. From the values so far it looks like the 330 pF are a little on the low side, but not much. To check for the effect of different loads I usually look at the output impedance.

For the output capacitor it is often better to have not just a single capacitor, but something like a small (e.g. 0.1-1 µF really low ESR one like a film or ceramic type) and one larger with a little more ESR (e.g. 0.1 Ohms range like a low ESR electrolytic).

You will have a hard time getting very good performance without a negative supply anyway. The OP usually does not need to be that fast, so even a LM358 might be good enough.

[blackdog]

Hi braddrew0, :-)

Next step, stop using these high value capacitors for C2, you already know this is not working 
You can play with C2 but not higher than 2,2nF.

This is a simple schematic and not all is well...
Place a capacitor between R2 and the collectors to ground, this make's de AC responce better 100 to 1000uF play with it is Spice.

And know the big step to make it better, place over R3-20K  a 0,1uF capacitor, tada!

Kleinstein already told you that two capactors over the output is better, start with 220uF in serie with 0,1 Ohm and a 2,2uF direct over the output.

Kind regarts,
Blackdog

[braddrew0]

OK quick update - I'll try to respond to your points tomorrow, but thanks, keep the feedback coming

I've added an input filter cap, gone to two output caps, a single protection diode and changed the simple integrator to a type 3 compensator. I played around with the equations from the second app note Steve provided above to try and set the poles/zeros I wanted, then I changed them all one at a time through a bunch of ranges until I found what I wanted. This is what I ended up with:



Circuit



Transfer Function



Impedance



Current pulse load (1mA to 2A at 1ms interval)


These look a lot better than the last ones - crossover frequency is about 3.7kHz and minimum impedance of ~150mohm at about 6kHz. Am I headed down the right path?

[Kleinstein]

The circuit diagram suggests a rather fast regulation. The impedance and transfer curve look rather slow. This might be due to the very low current flow that might make the output transistors rather slow. Especially the TIP140 with internal base-emitter resistors this can be a problem. So a something like a dralington configuration with separate transistors might be a better choice - this also allows for smaller emitter resistors, as the first transistor can be shared.

A maximum impedance of 150 mOhms looks about right, though it should not be much larger than the ESR of the damping output capacitor. But the frequencies are way to low. normally one should go fo something like a maximum impedance of something like 100 mOhms at about 100 kHz and something like 1 mOhm at 100 Hz. Also the output capacitor is relatively large (thus the reason for shifting things to so low frequencies) - this type of circuit should work with much smaller ones as well.
So the adjustment is not really good. The values for C4 and R13 look strange - so they should not have much effect at all. Usually C4 should be significantly larger than C2. R14 looks rather small - the rule of thumb has R14 at about 1/10 of R3.

The pulse response should use a longer Pulse, so that the final value is reached, usually something like a single 10 ms Pulse
(e.g. 10 mA - 1 A - 10 mA).

[braddrew0]

Thanks Kleinstein - R13 and C4 only seemed to slow the loop down, so I removed them and dropped R3/R4 to 4k/1k. With C2 at 18pF I could get a crossover frequency of ~50kHz, but this blew the impedance out. I'll try looking tonight for something that splits the darlington out. Thanks again

[braddrew0]

Hi blackdog - just to get back to you, that 0.1uF across the resistor divider was great! Thanks for the tip - I've been reading about type 1, 2 and 3 compensators based on the other posts, so I can see now where it comes from. Thanks once again!

AcHmed99 - wow, this is great info, thanks! I really wanted to learn a process for this in the future, and although I know how I got to where I am now (and I think I could repeat it), I haven't really worked out a straightforward start to finish method. I think you're right on my transfer function as well - my AC source is in a different spot from yours and from the picture you provided before... I've been putting mine between the feedback resistor and the opamp (so between R3 and U1 on my schematic) and measuring at the output. Now I have a bunch of questions if you're happy to answer:

1. In terms of process, are you recommending the following?

* Mock up the system using a type 1 compensator
* Measure the loop gain transfer function
* Based on phase margin at desired bandwidth, change to either a type 2 (up to 90 deg) or type 3 (greater than 90) compensator
* Select component values to give desired bandwidth
* Re-measure and adjust

2. With respect to measuring transfer function, both your circuit and the one from Cristophe's book have an LC filter on the output of the opamp (with high values). Is this required, and if so, what's the purpose?

3. Your transfer function measurement has a load on the output - is this required? So far all of my "transfer functions" have been no load.

4. How are you measuring impedance? I have been placing an AC current source at the output (again with no load) and the source travelling from ground into the circuit (I read this on diyaudio.com).

5. Can you expand on your comment about selecting the crossover so the output caps filter the undershoot?

6. Why did you select ~15kHz as the bandwidth of your design?

I'm sure I'll have more questions, but I'll take what you've written and see if I can rework my system. Thanks for your help, I appreciate it


EDIT: This document (http://powerelectronics.com/site-files/powerelectronics.com/files/archive/powerelectronics.com/power_systems/switch_mode_power_supplies/808PET22-eliminate-crossover-frequency-guesswork.pdf) has some great info which answers questions 5 and 6. I'll leave them here for anyone else.

[braddrew0]

I'm having a bit of trouble getting the loop transfer function to simulate correctly. I've split the darlington out into tip3055g driven by a small NPN (mmbt489lt1). I also crunched the numbers from that last link of what I'm after - with the 180uF output cap, to keep inside 5mV of ripple on a 2A drop, I need a corner frequency around 550kHz. Output cap ESR needs to be below 1.4mohm for this to occur. The figures in this schematic are from real components (although I need to parallel a few ceramic caps to get the 1.2mohm).

Current circuit/trasnfer functions look like this:





You can see I added the high value inductor/cap but I'm not convinced I'm getting the right transfer function? Here the purple line is supposed to be the loop transfer function, and the green line is supposed to be the power transfer function. Things I've tried:

* I had to bump the input voltage up significantly to allow it to reach max output voltage. With 26V in, it would only regulate to ~19V, then above then it broke down. The loop tf started at around -20dB and went down from there. If I fed 3.8V into Vref at 26V supply, it gave a loop tf almost identical to this one.

* I tried modifying all the transistor resistors (R9-13). They didn't really change anything.

* I tried replacing the mmbt with another tip3055 but it gave the same output.

* I tried changing the sense resistor R3, but this gave me exactly the same loop tf. This is part of what makes me think it's incorrect.

* I tried adding a type 1, 2 and 3 compensator, but each one only affected the phase of the circuit.

* I noticed the phase doesn't start at 180 degrees here - it's like the circuit is behind the 8 ball before it even starts.

* I tried changing the output (removing the cap, increasing and decreasing the load resistance). All produced a "worse" transfer function (ie <0dB all the time).

* I tried running a trans analysis to see if there's anything majorly wrong with the circuit. Apart from not quite reaching 20V out with only 26V in, I can see without compensation that the output oscillates slightly (~2mV) with a capacitative load and is reasonably stable under a resistive load.


Any other suggestions? 

[braddrew0]

And AcHmed99 - thanks once again... I bought the first version of Christophe's SMPS SPICE book about 7 years ago. I read it a couple of times and learnt "concepts" from it but I never pushed myself to learn the detail. I ended up donating it to charity a couple of years ago because I thought I'd never grasp the details. Big mistake! I loved his teaching style and I found it a lot more accessible than "academic" books on the subject. I think that's great advice to pick up some of his books now I'm absorbing more - thanks!

[braddrew0]

On the CD? Unfortunately no - we moved into a small apartment and I had a lot of books, they all needed to go

I'll place the order with Amazon today - in the mean time, I'll digest what you've given me. Thanks again

[braddrew0]

Thanks Achmed - this is great info, it's given me something to baseline with. I've put it through my LTSPICE and I'm getting different results....   




Here's the circuit and initial transfer function. I'm getting a bandwidth of around 15kHz (vice your 30) with a 127 degree phase margin?



Something slightly different I noticed - the output of my error amp is sitting a lot higher than yours at about 9.6V.



And lastly the pulsed load - this looks very different from yours. Yours looks like it has much higher fidelity than mine, but your recovery is much faster.

Unless I'm completely missing the mark, my results are close to yours but generally "worse"... The only component I can think that's making the difference is the opamp. What amp did you use? I tried simulating a simple switcher with this amp and it fell apart as well - might be time to find something different.

Thanks again, appreciate the help and effort you've gone to


EDIT: Just tried replacing error amp with LT1819 and LT1496 which are the fastest and slowest opamps in my library. Output on the pulse is exactly the same?

[Kleinstein]

There could be slightly different models for the transistors around. The TIP3055 is not only made by TI. A factor of 2 in the bandwidth can happen for different models. Especially the dynamic performance at small currents may not be the same in all models.

Usually one should add a small resistor at the emitter. This reduces the influence of the model and prevents possible instabilities at rather high frequencies. Also a resistor in parallel to the base-Emitter junction of the large transistors is a good idea to make the output stage a little faster turning of and behave better at low currents. A resistor (e.g. 50 Ohms range) between the OP and the transistor stage is also a good idea - real OPs don't like every load and simulations may behave different with a reactive load at the output of the OP.

LTSpice sometimes has trouble with convergence, if a circuit is at the edge of instability.

For adjusting the regulator loop for a lab supply one should use two cases:
A) the worst case condition to assume, which is something like a large low ESR cap (e.g. 10 mF with ESR in the mOhms range)
B) a more typical small capacitance (e.g. the one in the circuit)

You want stability (e.g. 10 deg. of phase reserve) in the first case, and good regulation in the second. 

[braddrew0]

I think you guys have nailed it - I re-watched a few of Dave's earlier videos where he does power supply simulation in LTSPICE (https://www.youtube.com/watch?v=iTxKCQYMHbY, and particularly were helpful) and he mentions a couple of times that the pass device's models are important. He even shows a couple of examples where they fall apart using built in models (LT parts and non-LT parts). The models I've been using are all from OnSemi, and you're right, they are very complicated compared to, for example, the models from Diodes Inc. It looks like they keep a database of all the relevant information which then generates the models for them - so every model has every parameter. Tomorrow I'll go through and find the simplest possible models to demonstrate proof of concept, then maybe try the complex model to make sure it doesn't give too outlandish results. it's a little bit frustrating because I feel I know how to attack the problem, but I don't know enough to tell if the errors are coming from my mistakes or the software's.... 

A couple more questions popped up today. Kleinstein - if I use a small (say 1 ohm) resistor on the emitter with a single BJT, is there any reason I couldn't use that same resistor for current sense?

And second question - I've been looking at schematics of other power supplies to see how they incorporate current control. One of them I found uses a PNP to short out the reference voltage to ground. Are there any design concerns with a topology like this?

Thanks!

[Kleinstein]

The resistor at the emitter can also be used for current sensing. This is even true if transistors in parallel are used at higher current.

However using the resistor at the variable potential of the output is not really easy. One viable way is a floating regulator circuit for the current control. One can also have the resistor at the low side of the load - the resistor is still in series with the load and has the same effect on the voltage control loop. This makes current control much simpler and voltage control only a little more complicated.

For combining voltage control and current control there are mainly three options:
1) using diodes (or similar) to set the output to the minimum of the two control circuits for constant voltage and constant current.
2) make the current control to turn down the reference voltage for the voltage control.
3) make the voltage control to set the value for the current control loop (I have not seen this type yet).

The later version tends to be a little slower, as the delay times of both loops add. As an advantage the switch over from current control to voltage control is generally well behaved.

[braddrew0]

I've never really considered putting the sense resistor on the low side of the load - I like that idea The only problem I can think of is that would mean that the negative output terminal wouldn't be referenced to the PSUs ground? I guess that may or may not be an issue, depending on how the circuit is implemented (ie I think that would be a big issue if you were using a mains supply in a metal case with the chassis connected to circuit ground - would be easy to accidentally connect the negative output to the case).

I understand that with "normal" loads (load impedance >> circuit impedance) that the low side sense would not need a large supply voltage and the inputs would be generally well behaved, but for a lab supply (where load impedance may be < PSU impedance for capacitive/inductive load) wouldn't we need to design the low side sense to the same specifications as the high side? Sorry if this is a dumb question - just trying to figure out exactly how to overcome the disadvantages in both cases

EDIT: Just in case I'm not making my question clear, if we select an opamp that covers the full voltage range of the output, and allows one input to be at Vdd while the other is at 0V, then most of the issues with high side sensing go away?

[braddrew0]

I've decided the final product is going to be slightly different - 0-24V, 0-2A - but I'm going to add a pre-regulator to keep the temps down. I'll give full details on what I'm thinking in the next couple of days. In the meantime, I've run a few more passes which I think are highlighting one of the issues.



This is the new circuit, which is very similar to the old one but I've switched to a PNP pass transistor. I've kept all the protection off for now (the base emitter diode, the collector emitter diode, any OVP/OCP/OTP) just to try get the simulations working correctly. LTSPICE let me run the circuit with no specific transistors selected, so I've compared that to using models. In terms of output, without selecting any specific models I got a rock solid 24V. By selecting components, that switched to severe oscillations of the order of around 200mV. So here are the transfer functions:




First one is no model, second uses models. As you can see, the gain curves are very similar however there is a significant phase boost around ~100Hz. By my calculations, the phase margin should be sufficient over the "model" transfer function to provide a stable output. I should mention as well, both transfer functions were run using a low resistance load.




These are the impedance graphs - no model then model. The no model case looks completely messed up, but the model case looks pretty good - the bandwidth (around 300k) agrees with the gain curves of the other two functions, and looking at the phase, the no model case appears stable whereas the model case appears unstable.

From this, the only conclusion I can come to is that the method I was using to calculate the closed loop transfer function on LTSPICE is insufficient. I'm going to keep playing with this to see if I can find a way to do it (there are a couple of "alternative" methods I've found through Google). Also, one other thing - something clicked when I was drawing this circuit. I'm not sure the 2.5ohm resistance as a load is realistic on the last model. Without current limiting, at 20V (now 24V) that should draw 8 (~10) amps, which is outside spec right?

[Kleinstein]

The default transistor in LTspice is a quite fast one, but not that far from a 2N3904/3906.
For the output transistor you definitely have to choose a proper model, as power transistors are usually significantly slower.

It's true that the shunt resistor to sense the current at the low side will give separate negative output of the raw voltage and for the final output. But usually this is not a problem if the raw voltage is not connected to ground.

The transfer function for the output stage should usually be taken for the worst case load. This is something like a large (e.g 10 mF)  capacitor with a low (e.g. 0) ESR and a current source to set the bias current. Here either small or large currents can be the more critical case. So you might have to test both 0 and 2 A.

The impedance graphs are also better with log scales. The curve for the case with models does not look that untypical - though unstable, as far as one can see in this scaling. The impedance curves should be done for both cases, with the large inductor in place (thus essentially open loop) and without it - that is the final circuit. The impedance in the open loop case determines how much minimum capacitance / RC combinations are needed to dampen the output. Together with the output caps they should have a well behaved impedance (less than +-90 degree phase shift, but no need for low impedance or much less than the 90 degree limit). The output impedance with closed loop (and compensation in place) shows the performance of the regulator and also should have less than 90 degree phase shift. Ranges where the impedance is not very low should also have sufficient reserve, thus should be better less than about 60 degree phase.

The output stage with a PNP power transistor might need resistors at the emitters of the transistors to make them more linear.  This type of power stage also has a slightly different characteristics and may need a type 3 compensation, to make the regulator work with all loads.  The resistor at the collector is of only limited use. For current sensing this would require to transfer the signal to GND or the positive supply. If you don't need high precision for the current regulation it would be better to have the resistor at the emitter side of the PNP.

[braddrew0]

Thanks Kleinstein - I've made those changes and they made a noticeable difference  I really appreciate all the help you've offered me

I think I've got most of the tools I need now to start working on the project I've been dreaming up - just need to spend the time trying to find what works and what doesn't I'm about to head away for a few weeks holiday, so this will be in the back of my mind. Hopefully I'll get a chance to put something on paper - I'll update all of you when I get back.

Thanks again to everyone for your help - stay tuned for big changes in revision C