First Bench Supply - Ripple/Noise Problems...

[MikeNye]

Hi everyone,

As per Dave's comments in the first LT3080-based power supply video, as a beginner, I've been working on designing my own bench supply as my first foray into analog electronics.

I'm working on a bench supply with the following specs:

• 0-30V Regulated DC Output
• 0-3A Constant Current / Current Limit
• Linear

I have chosen to use a series pass transistor driven by an op amp, rather than go with an 'all-in-one' style regulator such as the LT3080 / LM317 etc. This is mainly due to:

• It appears easier to get a 0V output with this configuration
• Hopefully, I'll learn more in the process... 

I have learned quite a lot from looking at Markus_B's design (https://www.eevblog.com/forum/projects-designs-and-technical-stuff/lab-powersupply-markus-take/), and also from reading the HP power supply handbook (http://cp.literature.agilent.com/litweb/pdf/5989-6288EN.pdf).

My design appears to work, however I have big problems with ripple and noise...

The schematic is as follows:

LTSpice schematics are here (http://jollyroger.narx.net/power_supply_ltspice_rev_G.asc) for those playing along at home.

The issue that I'm having is that there appears to be a lot of noise/ripple on the supply output in both CV & CC/CL operation.

I should note that I haven't yet breadboarded this circuit yet - I'm still working within LTSpice...

I can get CV operation to be stable when simulating if I remove "C1", "C2" and "C4", however this makes CC/CL operation very noisy.

With "C1", "C2" and "C4" in circuit with their current values, CL/CC operation is somewhat stable at higher currents (>1A), however at lower currents there is significant ripple.

Ideally, I'd like CL/CC operation to be stable enough to drive an LED with no current limiting resistor, without burning out the LED... I'd like to remove the ripple from CV operation so that it is stable enough to power sensitive digital electronics, such as microcontrollers / FPGAs etc. Is this too much to ask for on a beginner DIY bench supply? Do averagely priced commercial supplies regulate this well?

I've tried quite a few things to reduce the ripple, however everything I try seems to have issues or tradeoffs.

I've tried to add 2 & 3 pole low pass filters (using an op amp) between the output of R2 and U4, with a roll-off of 5KHz, however this severely breaks things and the output appears to be more like an AC supply than a DC supply, so I have abandoned this idea.

I've put in some very basic RC low pass filters (such as C5 & R13) - these seem to help a little, however these appear to slow down programming time...

I've tried putting a voltage follower (op-amp non-inverting buffer) followed by an RC low-pass filter before C2, however this appears to make things worse as well.

In my circuit, I think a lot of the noise/ripple is due to C4. As this capacitor is acting as a reservoir, if the system goes into current limit, there is a time where C4 will discharge and keep the output current higher than the set current. As a result, U6's output goes very positive and turns off U4. Once C4's charge is depleted, U6's output starts to turn off, which turns U4 back on. As there is time where C4 must charge back up, the current delivered to the load is still measured as being too low, which causes U6's output to turn fully off, which turns U4 fully on, and the whole process repeats.... As a result, I have added C1 & C3 to try and slow this process down a little. This appears to help but there still appears to be too much ripple/noise.

I've noticed on Markus_B's design, his current sense resistor is before his series pass regulator (LT3080). Perhaps I need to follow suit? However, would doing this cause an error in current measurement due to the base current of U4? Maybe I need to simulate this to see whether it would make much of a difference...

Also, I've noticed that op amp selection plays a large factor in the amount of ripple/noise. The LT1677 op amps that are currently in the circuit seem to result in the lowest noise/ripple....

I'm wondering whether I just need to build this thing, as the real world is different from simulation, as components are never perfect... I just want to try and get the design as correct as possible in simulation prior to building.

Have I missed something? Is my design fundamentally flawed in some way? I try to design a power supply, however seem to get a really effective long-wave radio transmitter instead...

Experts, I would really appreciate your assistance here, as I've been working on this for a few weeks and seem to be getting nowhere.

Thanks guys.

-Mike

[AndyC_772]

Hi Mike

Try this



Code here: clicky!

What you have here isn't really "ripple" and "noise" in the traditional sense. What's happened with your power supply is that the control loop is unstable and has gone into oscillation.

Control theory is full of hideous maths and obscure terminology, and if you ever find a really good, clear way to explain poles, zeroes, gain and phase margins, then do please let me know.

The nice thing is that often, in practice, you can get good results with trial and error - provided you have accurate models of your components, and you understand what it is that you're trying to achieve.

The one thing which I find de-stabilises a control loop more easily than anything else is delay. If the controller, which in this case is the op-amp driving the big transistor, is too slow to respond to an error signal (in this case, the difference between the output voltage and the required set point), then the output of the system has time to overshoot. The controller sees the overshoot but then over-compensates, and the error goes negative. The system oscillates.

There are two approaches to sorting this. One is to reduce the delay around the loop, ie. ensure that the controller can respond quickly enough to an error in order to correct it before it overshoots. The other is to reduce the bandwidth of the controller, so the loop gain is less than 1 at the frequency at which it would tend to oscillate.

With that in mind, I've made some changes to your circuit:

a) I've removed your R-C filters. They add delay, so they'll only ever make it worse. (That said, a very small C near an op-amp input can remove very high frequency noise which would otherwise make the circuit misbehave, but this is addressing a completely different problem. Such a filter should have a cut-off frequency that's much higher than the frequencies the circuit is normally intended to handle).

b) I've added a potential divider between the output voltage and the voltage control op-amp. This allows a capacitor to be fitted across the top resistor (R1), which increases the gain of the controller at ac, ie. speeds up its response to voltage errors at the output. In this particular circuit C2 isn't actually needed, but I'd definitely leave a site for it on your board when you make a real prototype.

c) I didn't have your transistor in my LTSpice installation, so I've picked a couple of others which seem appropriate. You definitely need a fast enough power transistor to keep the control loop from oscillating. If your transistor is too slow, a capacitor from the output of U1 to its -ve input will decrease the bandwidth of the controller and make it more tolerant of delay in the loop - though doing this will affect the transient response of your power supply.

d) to speed up the current limit circuit I've swapped the inputs to the op-amp, and replaced the output transistor with a diode. This eliminates the delay due to the output transistor on U6. I've also added a capacitor between the output of U6 and its -ve input; this decreases the bandwidth of U6 and prevents it from oscillating when the supply is in CC mode.

With my changes applied, the circuit is unconditionally stable But it's not without issues...

- Most importantly, the power transistor is going to get *very* hot. Hold <ALT> and click a component in LTSpice to plot its power dissipation.

- Output voltage is limited by the voltage from which you power the op-amps.

- I've not checked the transient response. Have a play and see what happens when the load changes suddenly. You'll certainly get a pulse of output current somewhat greater than the set limit when the circuit switches from CV to CC mode, because of the output capacitor if nothing else. I'd suggest keeping C4 fairly small, and putting the bulk of your smoothing capacitance on the 40V rail for this reason. (Lots of capacitance is the last thing you ever want on a constant current supply).

Your biggest problem will be heat in the power transistor. Draw any significant current from this supply and it's likely to burn out. My bench supply is an HP 6632B, which does 0-20V @ 5A - it's fan cooled and all the transformers and heat sinks inside mean it weighs as much as I do.

Many bench supplies overcome this problem by having a first stage PSU which can switch between different voltages depending on what output is actually required. For example, they may have a transformer with multiple windings that can deliver 10V, 20V, 30V and 40V depending on how many are actually connected. A separate control circuit monitors the required output voltage and switches in the correct combination of secondary windings so as to keep the voltage across the power transistor within sensible limits.

So, for example: if you set the PSU at 6V, the relay controller will select just the first secondary winding on the transformer, so the regulator is powered from 10V and the power transistor drops just 4V. If you then wind the voltage up to 17V, the relay controller switches in another transformer winding so now the circuit is powered from 20V, and the power transistor drops only 3V. Although rather crude, this form of pre-selection makes a huge difference to the amount of wasted power.

You can make a pre-selector to do this job with a few comparators and a bunch of relays - you just need a mains transformer with multiple secondary windings. Needless to say, be careful around the mains. By all means chicken out and use a big heat sink and fan instead, and save the clever stuff for the mk II.

[Rerouter]

i also began adapting my own from markuses thread, his is before to get rid of any voltage drop from the system,

if you want to do high side current sense realtivly easily an LT6105 is the chip i found to suit all my purposes with it (seperate supply, inputs can go far higher than supply)
but as your using a pass element a current sense follwing the output will get you some more accuracy,

also the golden rule to stabalising op amps is the add some capacitabce between the output and the inverting input, however you do run into the dillemma with the current limiting that it will overshoot if its more than about 10-20pF,

while on the vset it can be a whole lot higher, it will just effect the transient response, speaking of which, 100u on the output is kind of massive for a current limited supply?

[AndyC_772]

speaking of which, 100u on the output is kind of massive for a current limited supply?

...but handy if you want to check the circuit is stable when supplying a constant voltage to a load that includes bulk capacitance. Think of it as part of the load rather than the supply itself.

[MikeNye]

Hi Andy,

Wow, firstly let me thank you for your fantastic response. The internet never ceases to amaze me. This oscillation problem has been troubling me for at least 6 weeks or so, and only three and a half hours after posting the problem, I now have a detailed response that not only explains the issue, but a schematic totally solving my problem. If I ever end up traveling to the UK (or you ever travel to Australia), I am buying you a beer sir.

You mention control theory in your response - this is something I am interested in learning about. Can you recommend any texts or websites with information that helped you?

c) I didn't have your transistor in my LTSpice installation, so I've picked a couple of others which seem appropriate. You definitely need a fast enough power transistor to keep the control loop from oscillating. If your transistor is too slow, a capacitor from the output of U1 to its -ve input will decrease the bandwidth of the controller and make it more tolerant of delay in the loop - though doing this will affect the transient response of your power supply.

The TIP142 transistor I've been using appears to be slower than the transistors you've included in your updated design. When I simulate with the TIP142, I need to add the additional capacitance between U1's output and its non-inverting input. I'm using a value of 100pF, and this appears to work well and be very stable. Without it, at low output voltages it starts to oscillate again.

Also, while on this topic, how can one tell the speed of a transistor when looking at a datasheet? I have had a look at several transistor data sheets, and there appears to be no measure of speed...

d) to speed up the current limit circuit I've swapped the inputs to the op-amp, and replaced the output transistor with a diode. This eliminates the delay due to the output transistor on U6. I've also added a capacitor between the output of U6 and its -ve input; this decreases the bandwidth of U6 and prevents it from oscillating when the supply is in CC mode.

This is genius! Rather than having a transistor that pulls the base of the regulating transistor to ground, we're pulling the base to ground via the output of the op amp. If we're not in current limit mode, the output of the op-amp goes high, reverse biasing the diode and thus current does not flow. Fantastic. Would I need to add some load on the output of U6 before the diode to keep the op amp happy? For example, 10K to ground? I understand that op amps like to have some load on their output?

- Most importantly, the power transistor is going to get *very* hot. Hold <ALT> and click a component in LTSpice to plot its power dissipation.

Your biggest problem will be heat in the power transistor. Draw any significant current from this supply and it's likely to burn out. My bench supply is an HP 6632B, which does 0-20V @ 5A - it's fan cooled and all the transformers and heat sinks inside mean it weighs as much as I do.

Many bench supplies overcome this problem by having a first stage PSU which can switch between different voltages depending on what output is actually required. For example, they may have a transformer with multiple windings that can deliver 10V, 20V, 30V and 40V depending on how many are actually connected. A separate control circuit monitors the required output voltage and switches in the correct combination of secondary windings so as to keep the voltage across the power transistor within sensible limits.

So, for example: if you set the PSU at 6V, the relay controller will select just the first secondary winding on the transformer, so the regulator is powered from 10V and the power transistor drops just 4V. If you then wind the voltage up to 17V, the relay controller switches in another transformer winding so now the circuit is powered from 20V, and the power transistor drops only 3V. Although rather crude, this form of pre-selection makes a huge difference to the amount of wasted power.

You can make a pre-selector to do this job with a few comparators and a bunch of relays - you just need a mains transformer with multiple secondary windings. Needless to say, be careful around the mains. By all means chicken out and use a big heat sink and fan instead, and save the clever stuff for the mk II.

Holding "ALT" and clicking the component doesn't do anything for me... It just plots the current through the device. When I choose "Add Trace", is there an expression that I can enter that will give me the power dissipated?

Regardless, I hear you. I understand that in the current iteration of the schematic, U4 has to dissipate a *lot* of power when setting the output at lower voltages. I haven't yet implemented any sort of pre-regulation as I have been focusing on getting the regulation part of the circuit stable first. I have some ideas surrounding pre-regulation. Three ideas to be precise:

• Implement a switching pre-regulator as per Markus_B's design and as Dave has shown in his videos. I am wondering whether this will introduce high-frequency switching noise?
• Implement a way to switch between windings as-per your suggestion. This shouldn't be too hard to accomplish as you point out, but finding the right transformer might be difficult...
• Implement a reservoir capacitor before U4, and monitor the voltage across it. I would then implement some sort of circuitry to fire TRIACs (on the transformer primary) or SCRs (as part of the rectifier) at an appropriate time to keep the voltage of the aforementioned cap a few volts above the desired output. I like this approach as it should be less noisy than a switching pre-regulator... Mind you, this is probably the most complex way to implement pre-regulation... The HP power supply handbook has some great information on this, but this may be too much to bite off for a beginner...

- Output voltage is limited by the voltage from which you power the op-amps.

Is there a way around this? It shouldn't be an issue for this specific power supply, as the op amp supply voltage is slightly above the desired maximum output voltage. In a higher voltage supply, I can see how this would be a problem, but I'm not sure how one would overcome it... I suppose you could drive the base of the regulating element with the output from a class "A" style amplifier arrangement, allowing the base of the regulating element to be at a much higher voltage than the op-amp driving the class A amplifier.... Am I on the right track here? It might be better if I diagram this:

Or use this URL if you want to play with this 'live': http://www.falstad.com/circuit/#%24+1+5.0E-6+10.20027730826997+50+5.0+50%0At+400+208+448+208+0+1+-49.54324104623944+0.0063085032973824555+100.0%0Ar+448+192+448+128+0+100.0%0AR+448+128+448+96+0+0+40.0+50.0+0.0+0.0+0.5%0Aw+448+224+448+272+0%0Ag+448+272+448+288+0%0Aw+448+192+512+192+0%0Aw+400+144+400+128+0%0Aw+400+128+448+128+0%0At+352+224+400+224+0+1+0.6482182256972545+0.6545267289946369+100.0%0Ar+400+144+400+208+0+10000.0%0Ag+400+240+400+288+0%0Aw+512+192+512+352+0%0Ar+352+352+352+432+0+1000.0%0Ag+352+432+352+448+0%0Ar+352+224+304+224+0+1000.0%0AO+512+192+560+192+1%0Ar+352+352+432+352+0+10000.0%0Aw+432+352+512+352+0%0Aa+208+224+304+224+1+10.0+0.0+1000000.0%0Aw+208+240+208+352+0%0Aw+208+352+352+352+0%0AR+208+208+160+208+0+0+40.0+5.0+0.0+0.0+0.5%0A

So in the above circuit:
 - the op amp is single-supply (10V & ground).
 - 1V in gives roughly 10V on the output (there is some error there because I just bodged this up quickly - it actually gives 11V...)
 - Thus 5V in gives around 50V out (as shown)
Is it worth changing my schematic to have this sort of configuration for the regulating element U4? Perhaps this is something I will simulate just as a learning exercise.

if you want to do high side current sense realtivly easily an LT6105 is the chip i found to suit all my purposes with it (seperate supply, inputs can go far higher than supply)
but as your using a pass element a current sense follwing the output will get you some more accuracy,

also the golden rule to stabalising op amps is the add some capacitabce between the output and the inverting input, however you do run into the dillemma with the current limiting that it will overshoot if its more than about 10-20pF,

Rerouter, thanks for your comments. I had a look at dedicated high-side current measurement ICs. The problem is that I couldn't find a nice one in a DIP package - they all seem to be surface mount. One of my other design specs that I didn't mention is I'm trying to maintain 100% through-hole componentry to keep assembly simple for a beginner.

Thanks for your tip about adding capacitance between an op amp's output and inverting input. This is something I will keep in mind for future designs.

while on the vset it can be a whole lot higher, it will just effect the transient response, speaking of which, 100u on the output is kind of massive for a current limited supply?

...but handy if you want to check the circuit is stable when supplying a constant voltage to a load that includes bulk capacitance. Think of it as part of the load rather than the supply itself.

I understand. The supply seems very stable with 100u of output capacitance, however when actually building the supply I will probably drop this down to something much smaller (maybe 1u or thereabouts?) to try and keep output stable and decrease programming time... Unless there is a reason to have much more capacitance....?

Once again, thanks so much for your comments. I think it is almost time to start breadboarding.

Kind regards,
Mike

[AndyC_772]

If I ever end up traveling to the UK (or you ever travel to Australia), I am buying you a beer sir.

Just as long as we don't have to get into a discussion about which nation's beer is best, I'll take you up on that 

You mention control theory in your response - this is something I am interested in learning about. Can you recommend any texts or websites with information that helped you?

Sadly not I'm afraid, it's something I covered in a lot of detail on my university course, and my wife has reminded me that it's also the thing that gave me my first grey hair. I may still have my course notes, but that's all.

Also, while on this topic, how can one tell the speed of a transistor when looking at a datasheet? I have had a look at several transistor data sheets, and there appears to be no measure of speed...

There are specs for turn-on and turn-off time, but these aren't strictly useful because the transistor is partially on all the time - it's neither cut-off nor saturated. There will be parasitic capacitances between the terminals which will certainly have an effect, though these don't seem to be mentioned - they're usually of greater concern with FETs.

It may simply be that the transistor's bandwidth just isn't sufficiently well defined that the manufacturer wants to be drawn on the subject, or maybe it's intended to be used for on-off switching at fairly slow speeds. Either way, it wouldn't be the first time a data sheet hasn't included useful information.

Would I need to add some load on the output of U6 before the diode to keep the op amp happy? For example, 10K to ground? I understand that op amps like to have some load on their output?

Not sure where you heard that, I'm not aware of any reason to load the output of an op-amp as a matter of course.

The only reason I've come across is in applications that are very sensitive to crossover distortion. For the lowest possible distortion (eg. in audio circuits), amplifiers are sometimes used in such a way that they're always either sourcing or sinking current, and never switch between the two. This is called 'class A' operation, but you really don't need it in this case.

Holding "ALT" and clicking the component doesn't do anything for me... It just plots the current through the device. When I choose "Add Trace", is there an expression that I can enter that will give me the power dissipated?

That's odd, it works for me. The mouse pointer changes to a thermometer icon when it's over the body of the component and ALT is held down.

If that really doesn't work (and I can't see why it doesn't, I'm afraid), then you can always go back to good old Ohm's law and its derivatives. In this case, P=VI, so the heat being generated is equal to the sum of all the individual V*I contributions from each of the pins.

It's a pain in the backside to actually type the formulae, though, which is why there's the ALT shortcut. For example, the formula for the power dissipated in U1 is:

V(Vset)*Ix(U1:In+)+V(N012)*Ix(U1:In-)+V(Voa)*Ix(U1:V+)+V(N009)*Ix(U1:OUT)

They're all V*I terms, but the equation reads like a baud rate mismatch to me!

Implement a switching pre-regulator as per Markus_B's design and as Dave has shown in his videos. I am wondering whether this will introduce high-frequency switching noise?

That's a good idea. Noise in switching regulators is about 10% down to component choice and about 90% down to circuit layout. You might struggle to produce a low noise switcher without using a board with a solid ground plane; don't even bother on a breadboard or stripboard. But with a well laid-out PCB and carefully selected filter components, there's no reason why a linear regulator powered from a switched-mode supply can't be very quiet indeed. I designed one for a customer last year which ended up so quiet I couldn't see the switching spikes on my scope at all.

Implement a reservoir capacitor before U4, and monitor the voltage across it. I would then implement some sort of circuitry to fire TRIACs (on the transformer primary) or SCRs (as part of the rectifier) at an appropriate time to keep the voltage of the aforementioned cap a few volts above the desired output. I like this approach as it should be less noisy than a switching pre-regulator... Mind you, this is probably the most complex way to implement pre-regulation... The HP power supply handbook has some great information on this, but this may be too much to bite off for a beginner...

I've not come across this technology before, though most of my power supply work is in dc/dc converters rather than ac. It might be fun to simulate.

- Output voltage is limited by the voltage from which you power the op-amps.

Is there a way around this?

Sure. Power the op-amps with a lower voltage, then build yourself a simple voltage gain stage out of discrete transistors to boost their output voltage. Use potential dividers to reduce the voltages that the op-amps see on their inputs, like I've done with the input of U1.

Designing the voltage gain stage is left as an exercise for the reader (if only because right now it's beer o'clock here in the UK)

The supply seems very stable with 100u of output capacitance, however when actually building the supply I will probably drop this down to something much smaller (maybe 1u or thereabouts?) to try and keep output stable and decrease programming time... Unless there is a reason to have much more capacitance....?

No particular reason - but many loads have significant bulk capacitance across their supply rails in order to reduce noise and maintain a constant voltage even when the circuit draws pulses of current from the supply. I tested from no capacitor at all up to about 10,000uF just to check it remained stable.

[MikeNye]

Hi Guys,

Apologies for the delayed response - work has been busy.

With regards to plotting power dissipation - I currently run a Mac and am running LTSpice in Wine, which may explain why my ALT key has issues. I'll take a closer look at this on the weekend to try and get this sussed.

I read the link that AcHmed99 posted - this has some fantastic information about exactly the issue that I was originally facing. Unfortunately, I don't fully understand some of the context that the author discusses... He talks about bode plots, adding 'zeros' and poles. Unfortunately I didn't study electronics past first year uni and thus don't really 'get' this stuff, however I do understand that the end result of this is to reduce oscillation and make his control loop stable.

The first design that the author shows looks almost exactly like the design that Andy modified. The author shows a second design, where the current limiting works by reducing the Vset reference voltage by way of a low-side MOSFET to ground. The author states that this design is significantly more stable that the initial version.

This is sort of what I was trying to achieve with my initial design (https://www.eevblog.com/forum/beginners/first-bench-supply/), however ended up abandoning that design in favour of this current version.

I'm going to simulate both and do some stability testing.

I did notice, however, that the author uses a relatively large capacitance on the supply's output - 220uF. The author states (on page 3):

Between modes, the supply still behaves very well. The above shot was taken with the LED load in CC mode, and removing the LED to an open circuit. We don't want to try this the other way with an LED (from CV to CC), since the capacitor charge will fry the LED (I have done this accidentally...).

I am wondering whether professionally designed / commercial power supplies have some sort of method to drain the output capacitor when reducing the output voltage/current etc... Is this something that is typically designed into power supplies, or is it universally assumed that the power supply user is competent enough to be aware of such dangers and act accordingly?

I guess one could:

• Reduce output to 0V, 0A
• Use a dummy load or large wattage resistor to drain any output cap
• Attach sensitive device to supply (ie: LED)
• Program the PSU, starting with current, then voltage

...this way the power supply's output capacitor is drained, and by setting the current first, we ensure no overshoot when the voltage is set...

With regards to beers, I think both countries have some fine offerings. Theakston's Old Peculier is hard to come by down under, which is one of my favourites. Unfortunately, I believe the stereotypical Australian beer that Brits think of is probably Fosters, which is a shame. I'm not sure whether Little Creatures makes it over to the UK...?

Thanks again everyone. I'm learning a lot here.

Kind regards,
Mike

[MikeNye]

Oh, I almost forgot...

Andy, if you're still following this thread, I wanted to ask you about C2 in your schematic.

b) I've added a potential divider between the output voltage and the voltage control op-amp. This allows a capacitor to be fitted across the top resistor (R1), which increases the gain of the controller at ac, ie. speeds up its response to voltage errors at the output. In this particular circuit C2 isn't actually needed, but I'd definitely leave a site for it on your board when you make a real prototype.

With my limited understanding:

• At high frequencies, C2 will act as a short, thus allowing transients to pass (mostly unattenuated) to the op-amp
• At low frequencies, C2 will act as open circuit, thus allowing feedback signals to pass through the voltage divider R1 & R2

How did you come up with the value of the capacitor? Is there a certain impedance that you're trying to hit at a certain frequency, or do you just want to pass 'high' frequencies through?

Thanks.

-Mike

[AndyC_772]

I did notice, however, that the author uses a relatively large capacitance on the supply's output - 220uF. The author states (on page 3):

Between modes, the supply still behaves very well. The above shot was taken with the LED load in CC mode, and removing the LED to an open circuit. We don't want to try this the other way with an LED (from CV to CC), since the capacitor charge will fry the LED (I have done this accidentally...).

I am wondering whether professionally designed / commercial power supplies have some sort of method to drain the output capacitor when reducing the output voltage/current etc... Is this something that is typically designed into power supplies, or is it universally assumed that the power supply user is competent enough to be aware of such dangers and act accordingly?

To answer that question, here's what happens to the output voltage if I set my bench supply to 3.000V with a 10mA current limit, connect it to a red LED, and switch on:



This otherwise excellent bench supply takes about half a second to switch into CC mode and limit the output current at 10mA. Fortunately this particular LED was particularly cheap and nasty, and it has quite a bit of internal series resistance which limits the current. Even then, it does glow an amusing shade of orange until the current limit kicks in.

Interestingly, this supply has a "fast" mode available, which reduces the output capacitance - but it makes no difference to the start-up response. This suggests to me that the delay is caused by the control circuitry rather than being simply down to the amount of energy being passively stored in the output cap.

For what it's worth, I actually like a power supply to be able to deliver a decent current surge without limiting straight away. Plenty of products draw a substantial start-up surge, and they can even be damaged if their power source keeps dropping out. You can get into a nasty oscillatory state, where a load tries to draw a surge, the power supply current limits and reduces its voltage, the load turns off, power supply recovers... repeat until something overheats, which can be a matter of seconds. The same can also happen if there's too much inductance between a power supply and its load, but that's a rant for another day.

I'm not sure whether Little Creatures makes it over to the UK...?

Sadly not, unless someone would like to correct me

[AndyC_772]

Oh, I almost forgot...

Andy, if you're still following this thread, I wanted to ask you about C2 in your schematic.



How did you come up with the value of the capacitor? Is there a certain impedance that you're trying to hit at a certain frequency, or do you just want to pass 'high' frequencies through?

Since it's not actually required in this circuit, I literally just picked a very small value just to indicate that it might be beneficial to put a capacitor in that position. There's no science there!

If you experiment with other parts of the circuit and find it starts to oscillate, C2 is a component whose value you might like to play with. Values around 100pF to 1nF tend, in my experience, to be helpful. If you need more, chances are there's a problem elsewhere.

[MikeNye]

Hi Andy,

Thanks once again for your invaluable input and advice.

I appreciate that you took the time to rig up a test and perform a capture on your scope.

The idea of a 'fast' and 'slow' mode that changes the output capacitance seems like a good idea. I can see this being beneficial depending on the load you are driving at the time. I might add something to my power supply circuit that switches in and out different output capacitance depending on what response is desired.

I will post back once I have an updated schematic and have been through another round of simulations.

Thanks again.

Kind regards,
Mike Nye

[Stephen Hill]

I just want to say that this thread has been very informative and helpful.

In particular I learned how to control a high input voltage using low voltage op amps

Cheers
Stephen

[MikeNye]

Hi Stephen,

I echo your comments. Full credit goes to Rerouter, AcHmed99 and especially AndyC_772 for the awesome input. I have learned a lot so far!

-Mike

[T4P]

You know man, a not so good power supply is one that cannot limit current quickly ...

[AndyC_772]

Just by way of a follow-up, and since there's been quite a bit of discussion about power supplies here lately...

I rate the 6632B very highly, so I was surprised to see it staying in CV mode for quite so long after power-up. It seems to have few if any other vices, so I did a few experiments to try and characterise its behaviour a bit better. I can't believe this isn't something HP's engineers would have thought about.

So: after a happy afternoon connecting load resistors and watching the resulting traces, I have a conclusion:

If the load resistance is too low for CV mode - ie. if the current would be above the prescribed limit - then the supply will deliver about 20mC of additional charge into the load before switching to CC mode. This is fairly constant and predictable; it'll deliver an extra 200mA for 100ms, or an extra 3A for about 6ms. The product of [(extra current over and above the programmed limit) * time] remains remarkably constant.

How desirable that behaviour actually is might well be a topic for some debate. Fortunately most devices that are likely to be damaged by a temporary overload tend to be constant voltage loads anyway, and the start-up characteristic in CV mode is exemplary: smooth, clean, critically damped, and no overshoot whatsoever. Rise time is about 2.5ms, or about 500us in 'fast' mode. I'd happily set it to 3.3V and hook it up to a CMOS circuit without worrying for a moment about whether a transient was going to wreck something. The turn-off characteristic is almost as clean, and also has no overshoot whatsoever.

It's just the slightly slow transition to CC mode that might give cause for concern, but I think it's actually very well judged. Many loads draw a start-up surge (to charge up their bulk reservoir capacitors, usually), and a supply which can't maintain its output voltage while delivering such a surge can not only fail to work properly, but also actually cause damage.

Clearly there's circuitry inside the HP which is allowing a surge to be drawn, but is also controlling the maximum amount of energy that the surge is allowed to deliver.

Of course, a bench supply doesn't have to be this sophisticated, but these are all things to think about. I've certainly learned something!

[sorin]

try this
D1 and D2 are used to isolate voltage limiter from current limiter
use voltage divider R16, R17 do reduce noise.
Use C2 to reduce starting overshoot.
hope it helps

[AndyC_772]

Doesn't work for me

You've got a floating input on the current sense amplifier U3, and the current limiter doesn't seem to work. I don't have time to debug it properly right now, but D2 certainly looks backwards. With it this way round, the current "limit" circuit can only ever *increase* the output voltage.

[sorin]

you have right about D2
*U3 fixed (reupload)