MOSFET linear regulator circuit

[Kleinstein]

For the output capacitance of the linear stage, only ceramic caps could be a problem. They have very low ESR and thus don't provide damping. It may work if one of the caps has a series resistance (e.g. 0.1 - 0.5 Ohms range). Still a low ESR Al electrolytic is usually easier. Usually one wants a combination of some capacitance with low ESR (like 1-10 µF ceramic) and some with ESR (e.g. 100 µF low ESR electrolytic). The best size depends on the rest of the circuit: a slow regulation needs more capacitance. The current limiting shown below is rather slow anyway - so besides the physical capacitance, on transition to CC mode the supply will behave like having something like an extra 1000 µF or so anyway. So minimizing the capacitance would need a different circuit.

For the switched mode stage one might used only ceramics, but they also get quite large in volume / price, as one might need 50 V types, as the capacitance is reduced at relatively high voltage used. So electrolytic ones are still not such a bad option.

For the protection one could get away with just checking the full 6-8.4 V voltage - especially of one stays away from the extremes, which also allows for more cycles. One could also check both voltages separate - so 2 protection circuits, but no use for 4.

[VEGETA]

what do you mean by both voltages and 2 protection circuits? if you mean just monitoring the full pack voltage, then there are lots of ICs to do it but they involve using a fuse which is unwanted... I just want on off stuff. What IC do you think your suggestion fits?

Ok, so putting 100uF elec cap(polarized cap) plus 2 10uF ceramics on the linear output between the load only not including the shunt resistor right? and putting 2 100uF elec caps with some 10uF ceramics on the switching stage too.

I do want the transition to CC to be faster but if I removed the caps on the op-amps it won't be stable.

Any suggestions for smd mosfets to be used on both stages?

[VEGETA]

I've put a thought into this and reached to a conclusion that using IRFP250N is the safest option. Although I went for full SMD design, but I will most certainly do some manual wiring and harness. So why not just add one simple through-hole IC?! The harness is to connect the front and rear panels to the main board.

So, for a maximum of say 2W dissipation (1v drop * 2A max current), I thought of using one of these:

http://www.digikey.com/product-detail/en/advanced-thermal-solutions-inc/ATS-PCB1047/ATS2089-ND/5030467
http://www.digikey.com/product-detail/en/wakefield-vette/657-15ABPE/345-1220-ND/5068322

My housing is going to be small, like maximum height of 5 or 6 cm so I've gotta choose which one is the best. The smallest it is, the better.

Now for getting IRFP250N and the heatsink, I guess Chinese sources on Aliexpress is a good choice?

[Kleinstein]

For MOSFETs and similar more common parts aliexpress is a good source for fakes.  Depending on the power needed you could get away with a smaller old part (e.g. BUZ10, IRFP240) as well if costs are really critical. At least for more low cost parts there is a chance to get real ones if you don't go for the lowest price offers. Still do a quick test to check if they are real, or at least working well under power conditions. Normally I would prefer a more reliable source like an official distributor for semiconductors - however could be expensive in some countries.

If possible I would avoid loose cables - they can add hard to control parasitic inductance. At least keep them short and all three wires close together (e.g flat cable).

For cooling, I would consider mounting the FET to the case.

Keep in mind the gate drive may need something like 5 V higher than the output - so a second supply is essentially needed. The circuit also still needs to be optimized / adjusted. The plans shown in this thread are not yet ready and still prone to oscillations or other problems (like may not survive a sudden short).

[VEGETA]

I think I am fine with IRFP250N, Digikey offers it with 2$ or so. Aliexpress can give like 0.5$ per part if you bought 10 or more (I will test these too).

For cooling, the case is plastic or ABS so it won't do it. These 2 heatsinks are like 1.5$ so won't be a big problem.

xD, you understood me wrong! I don't want to wire the mosfet... I meant, since I am doing wiring between boards, why not get a through hole mosfet?! I wanted all-smd because of there was no need for manual work. Now, since manual work is a must, it is ok to pick through hole parts. The MOSFET will certainly be soldered hard xD. Now from the board to the output connector, of course there will be 2 wires because it is how it is done.

As for gate drive, I will put a 30v boost especially for the op-amps and the gate drive transistor. Now it can supply the needed voltage. BTW, this thing exist in the circuit already.

Oscillations... well, I put a short circuit on the output but it didn't oscillate, instead it produced a spark of 14A then went down to 2.2A which is set there. I used the "load1" and "load2" LTSPICE models to make loads like 10A or 50A but they do something that messes up the circuit.

They make the OUT+ less than OUT- which messes up the circuit... So does this mean I must make some reverse polarity protection circuit?

[Kleinstein]

The rather big sparc an a short is due to the relatively slow working current regulation. This is one drawback of this topology. It is relatively hard to get around that, though it could likely get better, e.g. with an faster acting fixed current Limit at about 3 A.

Some kind of reverse polarity protection is a good idea. The main case where it is needed is, if two supplies in series are used and the current limit is reached. Just current limit on the weaker one will not prevent the voltage to turn negative. The simple way is just a diode - though you might still get a negative -600 mV, but most circuits can survive that.

Heat sinks inside a plastic case have a somewhat limited performance. It might be OK with the preregulator and thus low power loss. It might be a good idea to have an over-temperature cut out.

[VEGETA]

I attached a new circuit showing a load that is 10R then suddenly shorted, however a 3A constant current limit is there... It actually worked! xD. It is not really a perfect circuit but I used the 2n2222 npn to switch the short circuit load off and on, thus it won't be perfect.

My aim is to put 2.048A current limit that is always on unless the user wants less. I want to do that by software of course.

Is there any oscillation or something else left to counter? I will think about reverse protection later, right now it is only one diode between OUT+ and OUT- (not ground), and while it is like this then I might put the output capacitance between these 2 terminals. However, is this gonna affect the circuit if I used elec_caps? or should I put elec+ceramic caps from OUT+ to ground?

As for heatsink, maybe it is enough to use this heatsink.

[Kleinstein]

The circuit is net yet ready at all - it is more like just a crude idea 99% still to do.

The output capacitance is missing (C2 going to GND is doing more bad than good). Changing that to 100 µF+0.5Ohms and 100 nF to Out- this at least makes the simulation to run through. Still the response is rather sluggish and stability is questionable.

For the simulation the load should be the spice element of current sink instead of a transistor. Its easier, more flexible and more powerful. 

[VEGETA]

Ok, what is left to be done in your opinion? so I can do some research to achieve it.

Output capacitance is fundamental thus I didn't put them yet to make simulation easier. C2 is for zener and gate, didn't think of it as output caps. What bad things will it do?

So putting 100uF elec cap with say 1R series res along with 0.1uF ceramic from out+ to out- is the best thing to do? this is what originally I wanted to do after listening to people.

I still don't understand where do the problems come from and how do I know them and solve them. You talked about this circuit is not ready and it still need 99% to be done... My only guess was that all is left is output caps and reverse protection. if there are more stuff, I am willing to learn.

well the transistor is not the true load there but I tried the current source and load but never worked properly as they made the voltage go negative

[Kleinstein]

One Problem is that the current limiting will need quite some time to react. When not active the OP for current limiting is all the way up to the positive limit and needs quite some time to come down: at least limited by the slew rate of the OP, but additionally limited by the capacitors in feedback. The rather slow discharging of the gate is a problem - with around 3 nF of the IRFP250 and 1 K this alone is around 3 µs of delay. So a first  step would be either a smaller resistor or maybe an extra PNP transistor to speed up turning the FET off as well.

Usually one adds a second, faster type of less accurate current limiting - like a resistor at the source side and a transistor to turn down the gate voltage fast. The source resistor also helps to limit the effective trans-conductance. So at high currents the resistor limits the effect of raising gate voltage. This makes the output stage less nonlinear.
Before looking at the loops one might want to check the performance of the output stage alone. So check how fast they are able to change the output current, when driving a low impedance load. Also the open loop output impedance is important - add output caps to make the output impedance well behaved (e.g. less than 90 deg of phase shift). Also check sensitivity to input ripple - the current circuit version is not good in that respect with the rather high capacitance IRFP250.

Than one has to look at the control loops, usually one at a time. One might also want to check if the cross over could be made faster. One way to do this is having the capacitors for Feedback from behind the diodes and not from before. This is somewhat similar to a simple kind of anti windup in a classical PID regulator.

For the voltage loop, the difference amplifier for sensing is somewhat tricky. One has to make sure the common mode amplification is not to the wrong side. For example a slightly to low value for R8 would cause a negative output resistance and thus instability in some cases. So the circuit might need adjustment for the output resistance to get a small, but positive value. The OPs choosen so far in the simulation are rather expensive, high quality ones. If lower speed OPs are used one might have to include that. A slow OP for the difference stage might cause troublesome phase shifts. So the capacitor to slow that stage down a little might already cause trouble.
For optimizing the loop one should use a current sink as a load. It work OK, unless the current limit is reached - a diode across the outputs would limit the negative voltage so that CC-CV transitions could be checked too. Looking at the AC response to a current sink as load give directly the output impedance and thus gives an easy check for possible trouble with certain capacitive loads.  Adjusting C1 and a resistor in series to C1 should give a first approximation that could work with easy load cases, that is avoiding load with high capacitance.

Likely there will be however purely inductive behavior for frequencies of below something like 100 Hz. In case of an extreme capacitive load (like a low ERS cap in the mF range), this would cause excessive ringing. Avoiding this would need an extra step of compensation adding phase lead and than another round of adjusting the compensation.  One has to test the loop with different DC currents and find a compromise that works in all cases. Usually something like 3 currents like 1 mA, 100 mA and 2 A should be enough. One a stable version is found one should also check transient response. With caps / delay at the wrong place one could end up with a good AC curve but still poor transient response.

The next steps are than the CC mode and finally the cross over response. As these interact with each other, it might be a good idea to first only use a more crude adjustment, than check if cross over is ok and only than do fine tuning at the end.
The CC mode loop is usually a little easier than CV, as the performance is anyway limited by output capacitance. So the adjustment could be more for good cross over than high output impedance. Depending on the required performance one might need more detailed anti-windup to get a fast cross over and little overshoot.

[VEGETA]

I am not sure I understood everything, but is there a book or something to help me understand? I will try to respond according to my understanding:

1- current limit:

Originally I used Dave's circuit of a transistor that pulls the base to ground, but the CV i guess was unstable. So you think this is gonna be faster and reliable?

the circuit works by the op-amps going to ground to activate the CV or CC stage, while dave's circuit is the opposite where the op-amp goes positive to do so. Since the final job is the same, what is the benefit here?

2- faster response:

I read that cc is too slow, why? is it because of filtering caps on the op-amps? these caps are necessary for stability as you know. removing them will cause problems of oscillation.

3-  gate resistors:

there is 22R and 1K. the 22r is for filtering (instead of ferrite bead) while the 1k is to discharge the gate as I read in eez-supply. I removed the capacitor from the zener to ground.

changing the 1k to 100 worked too while removing the cap didn't do anything so I guess it is better.

changing R3 to 1k from 10k worked well and also removing the other shunt filter made simulation faster (dunno about response). Here I am sure that my very first circuit had a stability problem in the CV loop itself, thus CC didn't work.

4- I connected the feedback caps before the diodes as you suggested.

I attached the circuit... If you can demonstrate an enhancement to it, I would be grateful!!!!

thanks!

[Kleinstein]

I did a few modifications to the circuit (circuit attached): The fet is changes to the smaller IRFP240 to get less ripple due to smaller capacitance.

The CC loop is not really optimized (only a few steps from transient). One might get away without the extra OP on the left. However it might be useful for measurement anyway. The CV loop is not yet checked for small currents so this might need a slower seting. A critical current would be something like 7 mA - just a little more than the current trough R2.

[VEGETA]

Thanks.

1- what is the purpose of R19 and Q1? there is already a shunt res and if you put this R19 then there is no need for the low-side sensing.

2- C2 and C18 from the mosfet gate to out-? I know that node is connected to the out+ but still...

3- it remains a wonder how you could pick the values for cc and cv caps and resistors...! especially odd values like R8 of 10.002k.

4- D4 is somehow understandable, preventing reverse voltage?

5- What is the purpose of R5?

what is left to do after this?

thanks!!!

[Kleinstein]

The circuit still needs a test and maybe adjustments at low currents (e.g. 10 mA range), both for CC and CV mode. Large transients also need testing (e.g. 2 A - 2 mA) - in rare cases these can cause (rather nasty - hard to calculate) oscillation. Also the CC-CV transitions should also be tested for a few more points.

The capacitors C8 and C2 are across the load. It is drawn a little strange, but it is not from the gate.

D4 has a dual purpose: it prevent to much reverse voltage for the transistors BE junction and it helps to discharge the output capacitor if needed (large transients). 

R5 is just a leftover - part of the load.

R19 and Q1 are a kind of emergency current limit (about 6A). With a good CV -CC crossover (capacitor from behind the diodes) Q1 might not be needed. R19 also helps with stability as it limits the "gain" of the FET at high currents. One might get away without it, it helped to get the first version running.

The funny value for R8 is there to show / check sensitivity on tolerances. In real life this might need a kind of trimmer to be sure to be somewhere in the 10K-10.005 K range (assuming the other resistors are accurate). It is adjusting the DC output resistance.

The capacitors for compensation of the CV modeare chosen iterative from the AC output impedance. R20 a little larger than R23 and so that R20*C4 is about R23*C11 to avoid another time constant. C1 started larger and was reduced until the curve looked good. The Transient response turned out to be ok from the beginning (as I new what the output impedance about has to look like).

[VEGETA]

Hi,

The attached file doesn't finish simulation unless I keep pressing ESC to view the results. Plus, you seem to use the "AC analysis" tab which I still don't know about it much other that bode plots of output vs feedback for each loop to check for zeros and poles. Perhaps this is how you picked the values for feedback resistors and caps? my concern is parts consolidation which is like using 1nf or something a lot rather than odd values that are used once for one thing. Is that possible in your circuit?

* transients:

Hmm is this by just transient response alone? like watching the time needed to switch between CC and CV? what danger does low currents do to this circuit? my guess is that CC will be pulling the output mosfet down a lot to achieve low currents... which might be bad for CV part as you said. Is this correct?

* Testing:

right now I don't have any of these parts, especially the mosfet and the npn controlling its gate. You choose 240p rather than 250p so I dunno if the bigger cap 250p will work nice or not, since it is more available i guess.

One bad thing is the op-amps! too expensive and won't be available unless you get them from digikey or any other official distro. I wanna choose other cheaper op-amps but I fear that the circuit will not work after all these efforts. EEZ-Supply uses TL07 op-amps but they have no LTSPICE models!

* extra current limit:

is this the same one as this image (eez-supply):

well, now I will use another 10 resistors (1 ohm value) to get this shunt res, let alone the switching regulator which must have it's own shunt res as well xD. 30 smd resistors are dirt cheap but takes place... lots of space xD. This is not a big problem though.

* "With a good CV -CC crossover (capacitor from behind the diodes)"

??

* "The capacitors for compensation of the CV modeare chosen iterative from the AC output impedance. R20 a little larger than R23 and so that R20*C4 is about R23*C11 to avoid another time constant."

You got all that from the AC analysis or what exactly (same as my first paragraph)?

if this will be a final circuit, then why not choose the values of R20,R23,C4,C11 to be the same since it is the same gain? is the reason for differing them that the value of R8 and R9 is not the same?

* "C1 started larger and was reduced until the curve looked good. The Transient response turned out to be ok from the beginning (as I new what the output impedance about has to look like)"

you mean the response time vs stability? bigger caps = more stable + longer time?

the stuff about knowing output impedance and curves is related to the AC thing I asked about so I won't repeat the question xD.

___

I learned that I must do AC analysis for all loops whenever I do stuff... to make sure I know what to do. this thing is new to me really, so it will be hard to learn... I just need to know what to do so I can know what should I learn.

always thanks for responding... always!

[Kleinstein]

The problem of the simulation sometimes not finishing / e.g. not really starting seems to be a little linked to the OP models. If this is a problem one could do the simulations with the universal model. This not as accurate, but usually good enough. One can there also adjust to being similar to any other OP. The difficulty in choosing a different OP could be that the circuit would need a single supply capable OP. So a TL07x would need a negative supply (e.g. -4 V). Speed wise the TL07x would be good enough, just drift could be a little on the high side for current sensing.

The AC response curve can help a lot. AC and transient simulations  are different ways of looking at stability. Some problems are more visible in the transient simulation and others are more visible in the AC simulation. I did the adjustment from the AC simulation. The transient simulation is than only a test to make sure there is no hidden problem that was not visible in AC mode.

The advantage of using the AC simulation is that one can directly see the output impedance and from that see if there is instability with any capacitive (or other) load impedance. In transient mode one would have to check with different output caps.

Also checking with low currents can be important, because the output stage gets slower at low current. So it is unlikely to have instability at intermediate currents if stability is good at high and low currents. Some circuits add an extra current sink to avoid the very low currents.

One could consolidate the BOM a little. The loop adjustment is not that critical / accurate (more like a factor of 2 in tolerance, except for the differential input)  and there are a few free points where the total gain is adjusted (e.g. resistor to neg. input). With the differential input stage one could get away with 2 of the same capacitor (e.g. 5 nF or 10 nF), but I have not really tested it. The resistors R20/R23 should be a little different, even with identical R8 / R9. The difference helps with stability and R20>R23 (even only a little, like with R8/R9) could cause trouble. The two points are somewhat related: R8/R9 are for the very low frequencies (< 10 Hz) and R20/R23 are for the higher frequencies (e.g. > 1 kHz).

The larger IRFP250 should also work. It might need a little lower discharge resistor and could have not that good PSRR. So ripple could come through stronger. So a smaller FET is somewhat attractive.

If the CC/CV cross over works really good one can get away without the extra current limit. In that case the gate/source zener should be chosen a little lower (e.g. 6-8 V), just in case. In my simulations the CC mode was fast enough, so the extra limit will not get activated.

[VEGETA]

Now, how to do ac simulation for each loop? or is it for the whole circuit?

You mentioned that R20>R23 can cause trouble while you actually put them like that xD. I prefer at least R8/9 be the same while also the caps be the same like 10n which could be used elsewhere like in the CC and CV comp caps.

I would need a rail-to-rail op amp to be cheaper than the one used here, but some of them are good but have one drawback which is bandwidth speed. like having 750k which is a lot less than say 2MEG typical opamp... dunno if this is an issue and also how to know for sure.

[Kleinstein]

For AC simulation the DC load current determines which loop is active at those settings. So it is either the CC or CV loop, but usually not both at the same time. One can run it with the whole circuit, or already start with a CV simulation before adding the CC circuit part. Ideally one should check the output stage alone first (with reduced circuit) - it turned out good in the simulation.

R20 should be larger (or equal) than R23 - sorry, for that. Just tolerance in the wrong direction could already cause trouble. So it is better to start with slightly different values and it helps to have the difference.

The OPs don't need to be rail to rail. Single supply should be good enough. For the voltage sense circuit, there is the option to use a slightly different circuit: instead of the differential amplifier for the sensed voltage one could use it for the reference voltage. This way one could get away with a less critical OP here (even an LM358 might work). It also depends on how the set voltage is generated.

The amplifier for the shunt should be reasonable quality (e.g. offset and relatively fast). One could get away without that OP altogether and directly go to the regulator OP.  Measurement could use a slower OP. Some ADC can directly measure at the shunt with still good accuracy.  Depending on the required performance the OPs should be reasonable fast - 1 MHz GBW is about the minimum, though I have seen similar circuits with just an LM358/LM324 (though using a BJT output stage). A really slow OP might need the extra current limiting.

[VEGETA]

So I can switch U1 and U3 with lm324 or the famous lm358? I can not find ltspice models for them, even tl07! the tl07 I got files for it and when i put them where they pointed out, it still didn't work and couldn't even select it.

For current measurement, since it is ground referenced (= 0v) I thought of removing the current amplifier and put it directly to the CC opamp but still I needed a way to make it x10 gain thus keeping it is ok too.

However, for voltage measurement, how about a simple voltage divider with /10 ratio and 0.1% resistors? max voltage of 20v = 2v from divider... but still it is not referenced to ground (0v) but for the out- terminal.. here I think a simple op-amp will do the job right?

the most important thing is to have an ltspice models for them to test them out.

can you point out how u did the ac analysis for this circuit? I need to spend the hole holiday to pick proper values for nearly everything to make a final circuit if possible.

thanks

[Kleinstein]

For the simulations one can just use the universal OP and set the parameters like GBW and slew rate accordingly. This way one could also test how fast the OP should be and look from there. With TL07x make shure the common mode voltage is right - so they would need an extra negative supply and are thus not a good choice. The LM358 is at least single supply, so it does not need a negative supply.

For the current loop using only 1 OP also has an advantage, as the 2 nd OP also adds delay. So using 2 OP can be a problem with slow OPs like the LM358. Still the LM358 for the current loop will be rather slow and has a rather limited slew rate: so in case of the sudden short, there can be quite some current spike.  So at least for the current loop, I would prefer a faster OP with single supply, GBW > 1 MHz and a slew rate of at least about 3 V/µs.

For the voltage control one could use just a voltage divider and thus only one OP for the loop. This would need a second OP to transfer the reference voltage / set voltage relative to the other side of the shunt. The advantage is two fold: the compensation circuit is a little easier (no two separate caps for phase boost) and there is no extra delay. So the OP can be rather slow.

For AC simulations the current sink as a load has AC amplitude 1. The interesting part is the output voltage - this than directly gives the output impedance. One can directly plot the difference from out+ and out- (drag with mouse).

[VEGETA]

After trying a lot, I modified the circuit to what is in the attachments. I didn't do any AC analysis unfortunately, but I applied the solution we discussed previously which is omitting the voltage sense op-amp and use a resistor divider instead.

I kept changing it and the comp filters but it kept oscillating as you can see.

Can you know why? what is the solution?

My guess is that the problem is the CV loop because its op-amp is the one that outputs ripple. I don't know how to fix this despite my trials. I can put a voltage follower op-amp but it won't be good enough. Just what is the difference between this circuit and the one before? I don't think that using the external limit shunt resistor is the reason too.

I would appreciate it if you told me how to learn how to debug these circuits using ac analysis or anything else needed.

thanks, as always.

[VEGETA]

In addition to my previous reply, I though of what you said about opamps and I found that most designs are using a good opamp for the current shunt only. The EEZ-Supply uses OP27 as I remember while Ian's design is using OP295 or something like that... while the rest of op-amps in eez supply are TL072D which is pretty normal.

However, Dave uses only lm358 (you can use lm324 too) but for the current shunt, he is putting 2 of them together as cascaded op-amps. This increases the bandwidth which might be the key to replace our very pricey LT1678.

Worst case is using one LT1678 (which has 2 op-amps) for the CC loop altogether, and using very traditional ones for the rest like CV and other stuff which can be ok with lm324 or lm358. One IC can have 4 lm324 which enhances the parts consolidation very much.


The problem with me now is that I can not simulate this in LTSPICE since it doesn't have models for these third-party ones. I tried putting TL072 model in specific folders but it didn't work (or I didn't do it properly/forgot something).

What do you think?

[Kleinstein]

For me the circuit did not show oscillations, but a common mode problem with the CC mode loop. With the current load, it got stuck at something like -700 mV at the output and the current limit part acting funny due to negative input voltage.

If one could avoid the common mode problem (e.g. limiting the load), the circuit would still have a problem with the current limiting. The differential amplifier would need really accurate resistors and could still show a not so good common mode suppression. Performance might be just acceptable for current limiting, but this will not provide accurate current regulation - the DC output resistor would not be very large. Assuming 0.1% resistor matching one would end up at around 1/1000 of the shunt or about 100 Ohms.

For the OPs one would like single supply OPs which can stand a high supply voltage. A possible, less expensive candidates would be OPA197 or OPA171. The amplifier for the shunt should be reasonable low drift and the current mode regulator might profit from a little more speed than the LM358 provides.

[VEGETA]

I played more with the circuit and found that the input supply was the problem, I made it variable a bit to simulate ripple but now I have chosen a steady value of say 21v which is typical... and now it regulates very well despite some issues like huge spike.

I wanted to make few modifications to the circuit, here are my suggestions:

1- Modifying the short circuit protection: well, how about putting it before the MOSFET? this will not give extra voltage drop on the linear stage.

2- Using high-side current sensing: In order to use my newer circuit which uses a voltage divider to sense the output voltage (- one op-amp), I must use high-side sensing. However, it still produced some issues like the one you mentioned which is common mode. Now, since I don't know the solution to this, I thought about what is in 3.

3- Using a high-side current sense amp: I found this part LT6106 which is somehow cheap (2$ from digikey) and a lot cheaper than a good op-amp (around 5$ for LT1678) as well as it is made specifically for the job = it can't go wrong.

However, it did went wrong lol. I tried their test circuit on their website [ http://www.linear.com/product/LT6106 ] and it produced correctly.

For our example, 0.1R shunt resistor... 100R input resistor and 1K output resistor gives a gain of 10. Which means 1A = 1V output from this opamp which is exactly like our CC loop, only better in terms of loop stuff and parts performance.

Now when I tried to put this simple circuit instead of the shunt comp op-amp, it didn't do well! it's output is so wrong with no indication why!!!

Using this part will make the design better (in overall) and will give us the freedom to choose other typical op-amps for the rest. With this, we only need one op-amp for the CC and one for CV which can be any nice cheap one like LM324.

Can you help with this? what is the problem in your opinion?

thanks!!!

[Kleinstein]

The current sensing amp only works if the voltage at the sensing shunt is higher than the level for the output resistor. So this would either mean one needs a negative supply or one would need a second shunt before the MOSFET. One would still need the resistor at the source to make the loop stable. Further the bandwidth of the LT6206 is not that high - this could cause a problem or limit the speed of current limiting.

If you really want to go with low cost OPs and still want good performance, I would go for an slightly different, not very common type: Have the current regulator floating. The downside is that you would need a negative supple (e.g. -4 V at about 1-2 mA) and a few more OPs/transistors - but most of them not critical, so cheap ones like LM358 or MCP6002 would do.

The trick is that a floating regulator for the current does not need to change its output so fast, as it is working from the gate to source (+shunt) voltage only. The downside is that one would need a kind of current sense amplifier (like the LT6206) to bring the measured current down to GND level and may need to bring the set current signal from GND potential up to the floating level. With modern low voltage OPs, it is possible the current regulator from the bias current sink.