| keantoken |
Hi.
I've been tweaking this design for quite a while now, and want to run it by the DIY community for feedback or suggestions. I have not built it yet, for lack of parts.
This isn't really intended for anything serious, I just started designing to see how well I could do. I figured that in the end I would have a nice lab supply with minimal ripple. Output is around 33VDC but can be changed by using a different zener diode. Adjustable Zener circuits work but not as well as using a single zener.
Rather than a capacitance multiplier, I decided I would go more the route of a specialized (super-sensitive) error amplifier keeping the output voltage steady.
If you want higher current you will need to lower the value of R3.
Q4 and Q6 act as a VERY sensitive feedback pair, which will react when current travels through the Zener diode. The 22 ohm resistor was a 1N34A germanium diode but... they don't exist anymore. The resistor works just as well here I suppose. Operating current through the 22 ohm is at about 20mA, but a .5W resistor is best because failure will likely result in oscillation.
C2 keeps the circuit from oscillating, though it seems from simulation that 100nF is over-conservative.
There is a hitch that I have not been able to work out, which is that the output is most steady after 0.2A, so ideally a class A or AB amp would have a standby current consumption of at least this much. Decreasing input voltage does not affect this. Any suggestions on how to fix this would be helpful.
I know that in the schematic has the input coming from a voltage source and not from a mains transformer. This is because I am lazy, not because I know nothing about safety. In an actual built unit, there would be fuses as well.
Simulated, ripple is about 1-2 mV at 2A, I haven't tested further than that. At 1A, ripple is about 400uV.
- keantoken |
|
|
| janneman |
Hi,
To get a real good feeling for the performance of the circuit, you should also test the ripple as a function of load current frequency. The ripple can be very low at 1kHz, but what at 5kHz, 10kHz, 20kHz?
Also, how does the output voltage change with changing input voltage? And what is the output ripple against the frequency of the input ripple frequency?
Jan Didden |
|
|
| Mooly |
Hi,
It might be OK in simulation but a few things stand out. Q4 what happens when it conducts- it looks like it can pull unlimited base current through Q6. R2 and Q3 ? not sure what you are trying to achieve there :) Connecting zeners across potentially "low impedance" points with high current capacity is asking for trouble, any spike will zap it.
Keep working on it, do you intend to build it :) :)
Edit, I would be nervous with this -- there is the potential for Q2/3/5/7 to put a virtually dead short over the unreg supply through all those B-E junctions. It would take only a brief "spike" to spell disaster. Q4 and Q6 "appear" to form a thyristor. Once Q4 is triggered into conduction Q6 will sustain it's base current whether or not D5 is passing current. |
|
|
| keantoken |
If Q4 conducts even a small bit, Q6 attempts to turn it hard on. Ideally, this would only happen if the unit started to oscillate since this would pull a lot on Q5s base and turn the whole thing off. However, I see the risk. On a previous version, this would turn on fully in the right conditions and draw around 2A. Those transistors would be history :).
| quote: | | Once Q4 is triggered into conduction Q6 will sustain it's base current whether or not D5 is passing current. |
It is a very sensitive configuration but it is possible to use it as a super-sensitive voltage sensor in the right conditions. Here, the regulating circuitry will have to react fast enough to cut off that voltage. It's a very precise feedback loop.
Adding a 100k resistor to Q6s emitter seems to work here without degrading performance, although if the pair still turns hard on I think those transistors might be blown. Hmm. I need a protection measure for that...
My initial idea was that Q2 and Q3 would act as a CCS, except that it also drives Q1s base, giving stable voltage across. Now it looks like Q2 and R3 just act a a current divider. I haven't deviated from this, though, since I've found nothing else that works as well. Believe me, I've tried.
| quote: | | Edit, I would be nervous with this -- there is the potential for Q2/3/5/7 to put a virtually dead short over the unreg supply through all those B-E junctions. It would take only a brief "spike" to spell disaster. Q4 and Q6 "appear" to form a thyristor. Once Q4 is triggered into conduction Q6 will sustain it's base current whether or not D5 is passing current. |
Hmm. Looks like we need a fast blow fuse and a sturdy case. :)
I don't know if thermal switches or fuses would be fast enough, to keep the transistors themselves from acting like fuses. :cannotbe:
Any ideas? I think discrete protection circuitry would be best... Hopefully my circuit isn't only good for a toaster. ):
At any rate, here's a AC analysis, using the load as the input, showing the current through the .5 ohm resistor, with the 100k resistor on Q6s base. I found that by using a pass transistor with MUCH less junction capacitance than the 2N3055 (415pF, WHAT!?), this was greatly improved. Unfortunately, that transistor is only rated for 1A, though it will still work in the simulator. Any recommendations for a good pass transistor with low junction capacitance?
- keantoken |
|
|
| sawreyrw |
keantoken,
I would suggest you run a transient (.tran) analysis of this circuit and look at the currents in the transistors. I could also give you additional feedback, if you like.
Rick |
|
|
| keantoken |
I remember you. :cannotbe:
I'll try not to be such a pain this time. Yes, feedback is fine. If I can't take the heat, that's my problem.
I have been using transient analysis and AC analysis side by side whenever it can help, as much as I know how. I look at the transient at about 10KHz, which is where this PSU operates the worst, and it seems that just plain junction capacitance is what does this. I still can't quite figure out why that bump is always around that area, though. Changing the value of C2 affects ripple greatly. Currently a value of 100p is best, from what it seems. Having C2 at too high a value isn't good, however, because it will trade output stability for input ripple rejection (which isn't what I want).
I've changed the output transistor to a ZTX something, with 7A max current, but the Vceo is 30V and the current Vceo is at max 27V, so I still need a better transistor.
Currently, output changes about 2.2mV from 1A to 2A load.
The image below is an AC analysis with a 1.25-2.25A sine load, probed at the output voltage. The other graph is the load current vs. output voltage at the worst operating frequency, 10KHz.
- keantoken |
|
|
| keantoken |
AHA!
Deleting the .5 ohm resistor cures it completely! The error was phase related.
When the load current rises, the output voltage lowers. But this is not because the regulation is faulty, because when the load current lowers, the output voltage is steady.
It seems that removing the .5 ohm resistor keeps the junction capacitance from becoming much of a problem.
Now the ripple at 10KHz is about 10mV.
It seems more prone to oscillate now, though, but it looks like 100p is enough to keep it under control.
- keantoken |
|
|
| Mooly |
Hi,
I will keep looking in ;) . I have the greatest admiration for you guys that design on the simulator ( something I have never got into ) . Ultimately your going to have to actually build it and do some real measurements. Looking at your latest circuit, have you added any rail capacitance to the output and local decoupling for R.F. stability. Does R6 need to be so low ? I can't just grasp the function of Q6. ( I can see what you are trying to do but the whole error amp looks to convoluted ).
Quite a good test (to do for real) is to place a power transistor (HEXFET is ideal) but any high gain high speed power Bjt will do across the output with a resistor that will draw say 2 amps from the supply. Drive the base or gate with a squarewave and look at the actual ripple and rail fluctuations. You can drive it from DC up to say 40 or 50 Khz. Very revealing. |
|
|
| keantoken |
I only expect to add rail capacitance to the output when I actually try and connect it to something. As for now, I want to get it as good as possible in a linear fashion, with as little as possible AC components.
And what exactly does 'local decoupling' mean? I probably know what it is but the jargon escapes me.
R6 is quite low but I found this was the optimal value by playing around in the sim. Curious that it also matches about the resistance of the 1N34A diode in the same situation...
Documentation on the Q4/Q6 pair can be found here although not in the way I use it. I find it weird that I have not seen a link to this site on DIYAudio once... Maybe everyone else knows something I don't?
| quote: | | Quite a good test (to do for real) is to place a power transistor (HEXFET is ideal) but any high gain high speed power Bjt will do across the output with a resistor that will draw say 2 amps from the supply. Drive the base or gate with a squarewave and look at the actual ripple and rail fluctuations. You can drive it from DC up to say 40 or 50 Khz. Very revealing. |
I will remember this one. Sounds like it's liable to make something explode though. I can just hear some cheap electrolytic start fizzing shortly before popping and smelling very very bad. I would actually prefer to be more gentle with my circuits! Something like that really scares me... But I guess I need some more experience to really know what to expect...
- keantoken |
|
|
| Mooly |
Hi,
"Local Decoupling" The output impedance of any series reg like this will increase with frequency. It just means adding something like a 0.1 mfd across the output to maintain a low impedance at HF. I still can not see what Q6 does other than form a thyristor as I mentioned earlier. As you had it in the earlier circuit it formed a "crowbar" across the rail but now with a 100 k in the emmiter --- what is it's function ? Transistors connected like this used to be available as type BRY39 and BR101 used for triggering of thryistor based PSU in old tellys etc. |
|
|
| keantoken |
Alright, thanks.
| quote: | | I still can not see what Q6 does other than form a thyristor as I mentioned earlier. |
You know what, you're exactly right... I deleted Q6 and got better results. :cannotbe:
I then ran through several different versions of the circuit. This is pretty amazing. Hopefully I haven't fallen into a simulator ditch here, because this is very nice.
Naturally, the more components you take out, the smoother the remaining devices work.
I tried replacing R3 with a CCS, to help input ripple rejection... I failed horribly, and got a better circuit from the experience!.
I deleted the CFP pair, and just hooked Q2 and R3 up to a new PUT pair, and whoah...
With the new circuit (attached) if I put the value of R1 below 30k, the ripple rejection OVERCOMPENSATES. Yes. The output voltage is actually an inverted version of the input...
But the higher I make R1, the less output ripple rejection...
So if R1 is below 30k, you trade output rejection for input rejection. If it is above 30k, you trade input rejection for output rejection.
Currently the circuit is in a very controlled state... By adjusting R1, you can have a little 120Hz ripple but virtually no output ripple, or you can have virtually no 120Hz ripple, but a little output ripple.
This simple circuitry is effective! In the simulator, at least. I really do need to build this thing. I don't have a good pass transistor though... Urgh... Must... Build...
Hmm. Would a 2SC3996 work as the pass transistor here?
- keantoken |
|
|
| Mooly |
Hi,
It's looking more conventional now. You are trying to regulate the voltage by having a transistor shunt base current away from the two main devices, Q1 and Q2 when the output exceeds a voltage determined by the zener.
As you have it now try removing Q5 altogether.
What does Q3/R2 do. It will work without these I think. Connect the collector of Q7 to the base of Q2.
Have you tried rearranging it bit. Remove the bits as above. Replace the zener and R5 with a pre set pot say 10k with the wiper to the base of Q7. Add a zener in series with the emmiter of Q7 to ground around say 5.6 volt. This will form a proper error amp, and you can adjust the output voltage with the pot. Also value of R1 at 30k seems high -- not enough base current under high loads. You can always add current limiting in afterwards.
With the simulator can you add the MOSFET or Bjt I mentioned earlier and see the effect on the output. |
|
|
| keantoken |
| quote: | Hi,
It's looking more conventional now. You are trying to regulate the voltage by having a transistor shunt base current away from the two main devices, Q1 and Q2 when the output exceeds a voltage determined by the zener.
As you have it now try removing Q5 altogether. |
Q5 is the trump card of the entire circuit... Q7 and Q5 form the error correction circuitry, and very effectively, at that.
| quote: | What does Q3/R2 do. It will work without these I think. Connect the collector of Q7 to the base of Q2.
Have you tried rearranging it bit. Remove the bits as above. Replace the zener and R5 with a pre set pot say 10k with the wiper to the base of Q7. Add a zener in series with the emmiter of Q7 to ground around say 5.6 volt. This will form a proper error amp, and you can adjust the output voltage with the pot. |
The fact is that we don't really know what EXACTLY Q3 and R2 do, but what they do, they do GOOD. Nothing else I've ever tried has beat this.
The problem with adding a POT as you said, is that the resistance will leech the high-sensitivity of the Q7/Q5 pair, along with the Zener, which effectively destroys the circuit's ability to regulate voltage as good as it does. This is the only reason I haven't added a way to vary output voltage easily.
| quote: | This will form a proper error amp, and you can adjust the output voltage with the pot. Also value of R1 at 30k seems high -- not enough base current under high loads. You can always add current limiting in afterwards.
With the simulator can you add the MOSFET or Bjt I mentioned earlier and see the effect on the output. |
At least as far as 2A, R1 is fine. The most I'll be driving with this will probably be Symasym, a 120W amp. What is really supplying the pass transistor with its base current is Q2. This forms a darlington pair with plenty of gain, so I don't really need a very low value to get high currents out of this circuit.
The problem is, I am not trying to make a 'proper' PSU. I'm trying something different because the circuit you're turning this into is about 100X worse than my original, when I simulate it. (I am not angry, I'm just trying to be honest).
After making these changes that you suggest, I really have nothing different from the conventional voltage regulator skeleton. It may be the underlying principle, but alone it doesn't do anywhere near as good as if I leave all the modifications on.
I have looked at and understood the design of the regulator you suggested I turn this into, which is why I'm trying to make something better.
I'm not angry with you, mooly. I'm just not sure you understand what I'm trying to do here.
I guess your alternative is more convenient, but what I'm going for here is accuracy. I can live with inconvenience if I get enough out of it.
Although, I haven't tried substituting the Zener for the adjustable zener circuit below...
http://www.tubecad.com/june2000/page3.html
I could use a POT in this and it would probably work better for this circuit than what you suggested. I still want to see what kind of performance I can crank out of this first, though.
EDIT: I have to go to sleep now... I've stayed up for about two days and a half without sleep. I really don't understand how. My brain isn't any slower (that I've noticed) than when I wake up. I didn't feel tired, so I just kept going... For two and a half days. :cannotbe:
But at any rate, even if my mind is not feeling tired, my body is. I must rest my body...
- keantoken |
|
|
| Mooly |
Hi,
It's really good to hear what you are trying to do and you should try things out. I know I used to :D .
Are you going to have a go at building it. |
|
|
| keantoken |
I am definitely going to build this thing.
But I don't have parts... I think my 2SC3996 will work (a high-voltage CRT deflection transistor from and old computer monitor :)).
I have a few 2N5087s, which are apparently good for PSUs, because of their low junction capacitance. But apart from that I don't have any other transistors as suitable as them, except for HF transistors from the old computer monitor, and using those things for this I think is asking for HF oscillation.
I don't have a Zener diode...
This is naturally a not humongous design because I am trying to design it so that I actually can build it, so this is a plus.
So yes, I will build the darn thing. :)
I just don't know when I'll be able to. ):
I can probably change the Zener to different voltages and it'll work just as well.
At any rate, back to the circuit.
I know that Q3 and R2 to regulate the Vbe of Q2, as this was what I designed it to do. R3 is just low enough to put a good .6V Vbe for Q3. Higher resistors cause worse regulation, so it looks like this is the sweet spot. The base current for Q3 is about 10-15uA, which I find is the place where most transistors will operate their best for lowest input distortion. So I don't think the Q3/R2 occurance is a flaw.
I simulated with a 1N750 4.7V Zener, at the same currents, and the regulation is still quite good! So I think this circuit will work for any voltage, as long as the devices are properly selected and R1 is say a 50K trimpot.
I will try simulating with the high-power transistor on the output as you suggest, and I will also try using the adjustable zener circuit and see what it does to the quality of output.
- keantoken |
|
|
| keantoken |
| quote: | | Connecting zeners across potentially "low impedance" points with high current capacity is asking for trouble, any spike will zap it. |
I believe I have found a solution :).
This solution does not only help with that one problem, however.
The solution is to place transistor Q4, and put the Zener across its B-C junction.
This makes the Zener super-sensitive, and puts it closer to its ideal breakover voltage. With this arrangement, a brief voltage spike would quickly be shorted by Q4, and then by the pass transistor. Because of the low resistance of R3, Q7 is also not as susceptible to voltage spikes.
Because of this added sensitivity, Q7 now draws less current, meaning more headroom is left for the pass transistor, meaning that we can further lower R1.
The Zener has significant junction capacitance, 220pF!. However, the 2N5089 only has about 4pF, and thus, even when HF ripple is enough to defeat the zener diode, this will still modulate Q4s current, and it will still regulate.
Also, I have found a better place for C2, the capacitor required to keep the circuit from oscillating. It's in a much more sensitive area of the circuit, which means it can be lower and have just as much effect as the old position.
With these improvements, the circuit now simulates with 200uV of line ripple at 10Khz. |
|
|
| Mooly |
| I am looking :) Build it !! Test it !! |
|
|
| keantoken |
Mooly, your test circuit suggestion is a VERY, VERY rough test! I now understand why it is as revealing as it is...
If the correction circuits aren't as fast as the risetime of the squarewave, you either get voltage dip, or a voltage spike, depending on how your circuit works. Thankfully, we get a voltage drop with this one.
However, the spike is apparently enough to cause the circuit to go into oscillation... I always know when my circuit oscillates because the simulator get reaaally slooooooow. :)
The square wave source is my own circuit, stemming from the PUT oscillator found on the webpage I mentioned earlier. It is a quick & Crappy (TM) solution, but it is very convenient when you want superfast switching times, at high currents. The circuit oscillates using the miller capacitance of the MOSFET.
At any rate, the result. The circuit operates as I expected it to, except for the oscillation...
The pattern shown exhibits a beat frequency in the decay rate of the oscillation, and I'm willing to bet it has something to do with the input voltage ripple. See how the frequency of the input ripple and the frequency of the load are so similar? The beat frequency of those two shows up in the output, because it has something to do with the circuit's ability to oscillate.
This means that either
1: At lower input voltages the circuit can facilitate more oscillation (the longer decay rate of the oscillation observed). Or,
2: The rate of change of the input ripple, in addition to the output pulses, causes stronger oscillation start, which causes the oscillation to last longer, e.g. longer decay rate.
Based on the observations, #1 appears to be the most likely...
So, I will next attempt to help the oscillation without altering C2, which would degrade performance. My first act will be to increase supply voltage, the most obvious considering the nature of cause #1...
I thank you for your test circuit, Mooly. It is very revealing even on the simulator, and it is a precious gem of knowledge... A lot can be learned and enhanced by using this circuit...
- keantoken |
|
|
| Mooly |
Interesting to see it as a simulation. It is a tough test, I agree.
I know and respect you want to try things out for yourself, I will just say look at Q5 Q7 and C2. Isn't this essentially (not quite I know but all the ingredients are there) the same as the PUT oscillator.
Regards Karl |
|
|
| keantoken |
EDIT: Oh, I didn't see you post!. I hadn't seen it that way... I'm glad you pointed that out. Yes, I now understand the circuit better. If C2 is too high, the circuit will definitely oscillate! The reason it doesn't at stable voltages is mostly because of R3... R3 lowers the gain of the PUT pair, so that it cannot react fast enough to cause oscillation. So if C2 is too low to absorb the spike if the PUT suddenly turns on, the circuit will oscillate. It will also oscillate if the capacitor is large enough to delay the feedback signal too much. It would have to be fairly large for the circuit to oscillate in this way (with the modifications below), however...
BTW, If this circuit works in real life as well as it does in the sim, how good is it compared to most PSUs posted here?
actual post:
Sorry for double post, but there's a 1-image per-post limit, apparently.
If you look at the above graph and this one, you'll notice the weird jagged things on the output trace. I'm not sure but I believe these are artefacts caused by simulation errors, and they happen when the sim's ability to compute is limited by the 32-bit maximum accuracy of digital processing. Apparently this test is so intensive the results are difficult for the sim to calculate... At any rate this used to happen a lot when I first got the simulator and was making horrendously flawed circuits... It used to confuse a lot because I didn't know what was happening.
At any rate, the problem with oscillation was fixed by increasing supply to 70V. So I narrowly avoided having to increase C2, which would degrade performance at high frequencies.
I will try and take pictures of the devices I will try to build it with, as I really do want to build it, even more so since I did a complete recal of my oscilloscope.
Unfortunately, I may not be able to... Is there anyone else who would be willing to build it?
- keantoken
|
|
|
| keantoken |
I have found another regulator that uses this idea here (PDF, page 4)... So I don't think it's too dangerous.
One might suggest putting a capacitor across R3 instead to prevent oscillation, but this is not the way as it actually increases the chances of oscillation because it is at the very most sensitive part of the circuit and easily causes much delay due to R3.
I would also suggest that this part of the circuit if not the whole thing should to be inside a Faraday cage.
Here are the current specs as simulated:
Output voltage (Vout): 33.5V
Vout Offset from 0A-2A (DC constant-current): ~50uV
Ripple at 2A: ~200uV
Line ripple with a sine-modulated load current between 0A and 2A at 20Khz: 700uV.
Max. Current rating is over 2A, but I have not measured much that far. A current limiting circuit will be necessary, because the circuit oscillates when pushed past its limit. The way to increase the limit is to increase R1. However, I do not know exactly how this will affect performance.
Also, the problem with the voltage rising with load currents below 0.2A doesn't exist anymore.
Attached are two graphs:
The first is the output ripple vs. frequency.
The other is the output trace with a load current modulation index of 2A.
PS: It's finally happened. I was staring at a resistor blankly for a few minutes and then I thought: Green-Blue-Orange... 56K... :)
- keantoken |
|
|
| Mooly |
Hi,
Your circuit -- I will build (lashup more like) and try it. I am only going to use a 0 to 30 volt PSU as a source and a selection of different voltage zeners for D1.
Walt Jungs circuit puts the reference in the emmiter side of the error amp, the output voltage set by the feedback network R861 and 863. It's similar- ish to yours but look how Q853 is connected (collector). |
|
|
| keantoken |
Thank you! :):):) I am saved.
Yes, I guess Q853 is connected differently... Hmm.
My biggest problem is that I'm only 14 (or 15? I forgot 0_0)and my mother doesn't want me connecting my circuits to the wall outlet. While it is damaging to my pride to reveal this, I would rather that those reading this not think I'm lazy. :)
I am contemplating making a 120V step-up converter, naturally of my own design since I can't find any of my NE555s and I only really have transistors, capacitors, and wire. Problem is that I won't really get enough current out of it to do any serious tests.
Once again, thank you.
- keantoken |
|
|
| Mooly |
Well out of interest, here is what happened. The output is a sawtooth the amplitude of which is set by the zener. See picture, this is 12 volts peak/peak amplitude at around 125 khz. The frequency varies as the input volts is altered.
Sounds like you need a proper stabilised, fully adjustable lab PSU and (maybe :) ) try something a bit less ambitious to begin with. An adjustable PSU was one of the things I made first, from a design in a mag -- many years ago now.
Providing you can get someone to check any mains wiring first, at some point you have to go for it and have the confidence that what you have done is safe and correct.
Good luck with it all
Regards Karl |
|
|
| keantoken |
What components did you use? It looks to me like R3 was disconnected. In this circuit it is important to use components with as low parasitic capacitance as possible... I am currently trying to build it. I managed to pull a 12V zener out of a computer PSU, so it will be powered by 24V out of four 6V lantern batteries.
I'll play around with it and see if I can make it work... And if not find out why it doesn't work.
- keantoken |
|
|
| Mooly |
I used TIP41A for the pass transistor and BC546 and BC307 for others. R1 initially at 82 K . With a 24 volt supply the regulation was poor under load ( I used 15 ohm as a load ) and R3 was 27 ohm. Reducing R1 down to 10 k improved the regulation greatly.
At 82 K the output fell by a volt or more when loaded with 15 ohm.
The only way to stop the oscillation ( at a basic level without adding caps etc) was to remove Q5 and connect the collector of Q7 to the emmiter of Q3.
Regards Karl |
|
|
| keantoken |
Hmmm...
I think it is a good idea but when it gets to it the PUT pair is just to sensitive to be used in this way. I'll keep working though, and see if I can figure something out... It worked great in the sim though. :)
Thanks for your help, mooly.
- keantoken |
|
|
| sawreyrw |
keantoken,
The "PUT pair" is really more like an SCR, because the on resistance of an SCR is much lower than a PUT.
This circuit will inherently oscillate due to the latching action of Q5 and Q7. When these transistors turn, on the base emitter junction of Q3 becomes forward biased and the emitter current of Q2 becomes Beta_Q3*(56-2.8)/R1. In addition, the base of Q1 is pulled low and the zener no longer conducts. Then the cycle repeats. C2 and the natural response time of the circuit components will determine the oscillation frequency.
In order to get this circuit to work, delete Q5 and increase the value of R3. Q3, Q4 and R2 aren't required either. I know, this looks just like any other seires pass regulator.
As another point all power supplies have some fairly large capacitor right at the output terminals.
Rick |
|
|
| sawreyrw |
Keantoken,
Ops, I made a minor error. When Q5 qnd Q7 turn on, the emitter current of Q2 will be limited to Vbe3/220 or about 3 mA.
The rest of what I said is correct.
Rick |
|
|
| keantoken |
Okay, what you say makes perfect sense. I only tried to use the PUT pair in this way because I observed (on the simulator :P) that if the base current was regulated precisely, it would not latch.
I've just got some perfboard from Radioshack and some more transistors to smoke. :) Plus some silver-bearing solder, and a 2N3055 that maybe with some persistence I can rig into a PSU of my own qualifications. :D
So I'll be experimenting a bit more with real life. :) :)
A soldering iron is still on the list, however. For now I have to make do with a butane microtorch.
I think I'll start by making myself an LTP with two transistors and a CCS and go from there. Learning should be much easier now that I know how to use my oscilloscope.
I'm sorry if I'm a bit pesky, but strangely enough I can only learn at my own pace. Now that I've finally gotten comfortable with that fact, maybe I can finally learn something. :)
- keantoken |
|
|
| lineup |
| quote: | Originally posted by keantoken
Hi.
I've been tweaking this design for quite a while now, and want to run it by the DIY community for feedback or suggestions. I have not built it yet, for lack of parts.
------------
- keantoken |
Linear Pass transistor regulator - my design
This basic model posted below is what I usually begin with.
When designing my discrete regulators.
it has
- low voltage drop, can be as low as 0.05-0.10 volt at lower currents.
- very good regulation at different input voltage levels
( because reference is fed from output voltage! see my next post attachment, for this feature ) |
|
|
| lineup |
Here is one full implementation.
The trick here is the R1 = startup 1 Mohm resistor.
After this the reference is biased from output precise voltage level.
Via the diode D1.
This very version is for regulating extremely precisely from a 9 VDC battery.
Which can have a voltage going from 9.60 ... downto ~ 7.80 volt
when battery is close to empty.
Notice :cool:
7.57 Volt in ... and ... 7.50 Volt out ... at 20 mA output.
Suitable for hifi Op-Amp circuits, for example.
Lineup |
|
|
| keantoken |
Hi lineup. :)
Hmm. I've seen regulators using an LTP as a comparator, but for some reason I didn't like the idea... I think I'll abandon my previous design. It'll stay in my archives for interest, though...
At any rate, I coughed this up shortly after reading your post. D8 is to cancel the extra voltage drop of Q8 in the voltage reference, with D6 to equalize the currents in the LTP. C10 is required to keep the circuit from oscillating. :/
This is the first thing I though of. The CCS of the LTP is powered from the voltage reference. I'm not sure if Q9 is needed, but it extends the HF response of Q10, which is why it is there.
Is my logic correct so far?
At any rate, thanks for the circuit.
- keantoken |
|
|
| lineup |
| quote: | Originally posted by keantoken
Hi lineup. :)
Hmm. I've seen regulators using an LTP as a comparator, but for some reason I didn't like the idea... I think I'll abandon my previous design. It'll stay in my archives for interest, though...
At any rate, I coughed this up shortly after reading your post. D8 is to cancel the extra voltage drop of Q8 in the voltage reference, with D6 to equalize the currents in the LTP. C10 is required to keep the circuit from oscillating. :/
This is the first thing I though of. The CCS of the LTP is powered from the voltage reference. I'm not sure if Q9 is needed, but it extends the HF response of Q10, which is why it is there.
Is my logic correct so far?
At any rate, thanks for the circuit.
- keantoken |
Your regulator is rather advanced, compared to my circuit.
You fead reference from INPUT voltage. I from the Output.
This should give better line regulation for me. ( in-sensitive to input ripple and voltage variation )
D1, 1N4148 is the trick in my circuit. Very much Nice feature.
As I wrote in my post.
| quote: | When I tested that circuit in Sim.
I adjusted for 7.500 Volt at like 8.000 Volt input.
Using 20 mA load.
Not until I got downto 7.560 Volt input, the meter shows
7.499 Volt output ( ~ 0.01 % change )
Now I tested to raise the input voltage. Same load 20 mA.
Not until I came to 30 Volt input level,
the meter flips from 7.500 to 7.501 Volt ( ~0.01 % change )
This means, my circuit has an ENORMOUS Line Regulation.
Necause the bias of Reference, is al the time coming
from 7.500 .... the output |
Load Regulation, improves the higher GAIN we have.
This is also the reason I have added a PNP Driver to my output BD140.
I use only one output transistor (PNP). You use 2 NPN followers.
This will theretically, give you better load regulation. ( in-sensitive to LOAD current variations )
On the other hand, my circuit was itended for minimum voltage drop, from a battery + low current operation.
To my circuit we can add a Power Transistor (or Darlington, as you do )
as a follower.
This give +0.7 Voltage dropout voltage, but give out considerably higher current.
Your circuit will work, keantoken.
You may perhaps simplify it a bit.
------------------
Credits to you, for using a somewhat REAL SUPPLY ... for simulation.
We have guys :D at forum, like PMA etc. that posts horendous figures simulations.
They have just not realized, that the Biggest error source to their sims
is that supposing Ideal Voltage Soure
while using same Ideal Supply for Input VAS + Output Power stage
will screeeew their figures.
==========================================
:cool:
I attach what I use, when I want some better Reality, than PMA.
A simulated REAL Power supply.
Using numbers in the transformator Inductor core,
that I have measured on one Real Trafo I have.
Lineup regars |
|
|
| keantoken |
| quote: | | D1, 1N4148 is the trick in my circuit. Very much Nice feature. |
Okay, I give up. What does D1 do?
- keantoken |
|
|
| Mooly |
| I know what Diode D1 does :D :D. Think about it ?? Where does the reference get its supply from :) |
|
|
| keantoken |
| quote: | | I know what Diode D1 does . Think about it ?? Where does the reference get its supply from |
I know that, anyone who spends time on a regulator project usually does this. But I thought that there was something about the voltage drop caused by the diode or maybe its characteristics... Temperature compensation?
At any rate, I just put this together. It's actually no different than my first circuit except that it's simpler. It seems to work just as well too, at least in the sim. I've got it built and it's running on a 24V 4-pack lantern battery PSU. I'm not really sure if it's working correctly, I just know that I get some voltage when I flip it on. Probably something like 0.6V... At least it doesn't oscillate. :)
I actually fried everything but the 2N3055 when I first turned it on... Output is between ground and the collector of the 2N3055... Notice where ground is... I only did this so I could measure values on the sim easier.
- keantoken |
|
|
| keantoken |
It works! Output stable at 13.2V into 1.2K load...
I've yet to test very far, but it looks like Q3 has problems firing at random times...
If someone else wants to test, be my guest. Hmm. I need a variable current source for testing load... How much current can a breadboard take? That would be very useful about now...
- keantoken |
|
|
| keantoken |
| With my oscilloscope at the 1mV/Div setting, I can't see any difference in noise level between when the circuit is on and when it is off... |
|
|
| keantoken |
I'm multiposting, Mooly style. :D
Something's getting hot... Hot enough for me to smell... How much current does it take to heat up those small black transistors?
- keantoken |
|
|
| Mooly |
| I am still looking --- just don't know what to say :) |
|
|
| lineup |
| quote: | Originally posted by keantoken
I'm multiposting, Mooly style. :D
Something's getting hot... Hot enough for me to smell... How much current does it take to heat up those small black transistors?
- keantoken |
I use two 220pF caps to stabilize my regulator.
In a real amplifier such stabilizing compenastion may need more cap values.
further, there are most probably several other ways, than the way I use
to get regulator stable.
See my posted schematic above. For those 2 x 220 pF.
Now, as with any other amplifier using negative feedback with high gains
... the higher the gain .. the more capacitance may be needed to compensate VAS.
Actually I have used as high values as 1-2.2 nF in some such real life regulators I have built.
regars, lineup |
|
|
| keantoken |
I see...
At any rate this latest version seems to WORK. I don't know if it works WELL. But I guess that testing will be for another day, when I feel up to it.
Right now I've got another project going, an extremely high-Z MC pickup. I just smoked a 22ohm resistor. Pretty soon I'll be able to tell what I'm smoking by the smell, or maybe even taste. :D
:(
Luckily my three remaining 2N5088s are still alive. :)
- keantoken |
|
|
| sawreyrw |
keantoken,
The last circuit you posted should work quite well (except the input voltage is way too large). Good for you.
You could simplify the circuit be eliminating Q1 and moving the zener diode to where the collector and emitter of Q1 were connected. I would also increase R1 to 220 ohms. You want R1 to be small enough to bias the zener off its knee, but making it too small just wastes power.
In general zener diodes are not precision devices. Except for zeners in the 6.2 volt range, their temperature coefficient is large as well.
Rick |
|
|
| keantoken |
Thank you.
| quote: | | In general zener diodes are not precision devices. Except for zeners in the 6.2 volt range, their temperature coefficient is large as well. |
Through reading some things on this forum about CCSs, I've pretty much come to that conclusion. According to tests that were made, IR LEDs are best to keep a CCS stable when biased at about 20mA. I'm not sure what exactly is involved with switching LEDs out for zeners...
But at any rate, my reason for using Q1 as I did was so that minimal current would be running through the zener. That and from looking at the model, this zener has about 150pF of junction capacitance! So I think using Q1 is beneficial in the way that it increases the sensitivity of the zener, and makes total junction capacitance not more than the Cje of Q1.
Also, what if this oscillates horribly? What do you think would be the best way to prevent oscillation?
- keantoken |
|
|
| sawreyrw |
Keantoken,
As I explained, you should have a few mA (3 mA) through the zener to get it off the knee. Please elaborate on your comments regarding capacitances. How does the capacitance of D1 increase the sensitivity of Q1?
I simulated the circuit I described and it has a little "peaking" in frequency response, but it is stable. A transient analysis also show this.
Rick |
|
|
| keantoken |
| quote: | | As I explained, you should have a few mA (3 mA) through the zener to get it off the knee. Please elaborate on your comments regarding capacitances. How does the capacitance of D1 increase the sensitivity of Q1? |
If I may talk like a textbook for a minute (sorry, it's easiest for me to explain this way. I'm not trying to act professional),
Looking at Q1 like an amplifier, Q1 will increase the current swing when D1 starts to conduct (as well as slew rate). Since the input (zener) and output (collector) paths are kept separate, the amplifier operates at open-loop gain, if you neglect the rest of a circuit working as NFB. The high parasitic capacitance of D1 theoretically will degrade the performance of the circuit since it will bypass the NFB (if you now look at D1 as the NFB for the rest of the circuit) and will make Q3 act at open-loop gain. So since Q1 has a Cje of say, for a 2N5088, 14p, this means that the parasitic capacitance ('looking' into the emitter of Q1) can be no larger than 14pF. This was what I was trying to say.
I think if anything, the stopper with the above is the enormous Cje of the 2N3055. This makes optimizing for HF stability pointless.
At any rate, my theory with Q1 is that it will increase the slope of the zener knee to a point that it is useful. Biasing the zener elsewhere than this point can make the circuit vulnerable to parasitic fluctuations like temperature, and can cause less stability in output voltage. Also, I'm assuming that the voltage drop across the zener will wander with temperature if given a specific bias point, eg 3ma, while the actual point where the current begins to rise should be more solid. I don't know if this is correct.
As a note, I uploaded that version because it was the only one that was stable. If I change any of the components in the sim, it will ring like ****. This is why I was asking about oscillations. If the circuit is this sensitive to components, I don't know if I want to risk relying on simulation.
- keantoken |
|
|
| sawreyrw |
Keantoken,
Try this.
Version 4
SHEET 1 1104 680
WIRE -96 16 -144 16
WIRE 48 16 -96 16
WIRE 144 16 48 16
WIRE 176 16 144 16
WIRE 464 16 176 16
WIRE 544 16 464 16
WIRE 672 16 544 16
WIRE -96 48 -96 16
WIRE 48 48 48 16
WIRE 464 48 464 16
WIRE 176 96 112 96
WIRE 288 96 176 96
WIRE 672 96 672 16
WIRE 288 144 288 96
WIRE 464 144 464 128
WIRE 544 144 544 16
WIRE 144 160 144 16
WIRE 48 176 48 144
WIRE -144 192 -144 16
WIRE 288 240 288 208
WIRE 432 240 288 240
WIRE 464 240 464 208
WIRE 464 240 432 240
WIRE 544 240 544 224
WIRE 544 240 464 240
WIRE 672 240 672 176
WIRE 672 240 544 240
WIRE 144 288 144 240
WIRE 224 288 144 288
WIRE 144 304 144 288
WIRE 48 352 48 256
WIRE 80 352 48 352
WIRE -144 432 -144 272
WIRE 48 432 -144 432
WIRE 144 432 144 400
WIRE 144 432 48 432
WIRE 288 432 288 336
WIRE 288 432 144 432
FLAG -96 48 0
FLAG 432 240 out
SYMBOL npn 224 240 R0
SYMATTR InstName Q1
SYMATTR Value 2N3055
SYMBOL npn 80 304 R0
SYMATTR InstName Q2
SYMATTR Value 2N2219A
SYMBOL pnp 112 144 R180
SYMATTR InstName Q3
SYMATTR Value 2N2907
SYMBOL zener 304 208 R180
WINDOW 0 -53 44 Left 0
WINDOW 3 -124 -1 Left 0
SYMATTR InstName D1
SYMATTR Value BZX84C12L
SYMBOL voltage -144 176 R0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V1
SYMATTR Value 24
SYMBOL res 160 0 R0
SYMATTR InstName R1
SYMATTR Value 230
SYMBOL res 32 336 R0
SYMATTR InstName R2
SYMATTR Value 1k
SYMBOL res 128 144 R0
SYMATTR InstName R3
SYMATTR Value 500
SYMBOL cap 448 144 R0
SYMATTR InstName C1
SYMATTR Value 100µF
SYMBOL res 528 128 R0
SYMATTR InstName R4
SYMATTR Value 500
SYMBOL res 32 160 R0
SYMATTR InstName R5
SYMATTR Value 100
SYMBOL current 672 96 R0
WINDOW 123 24 116 Left 0
WINDOW 39 0 0 Left 0
SYMATTR Value2 AC 1
SYMATTR InstName I1
SYMATTR Value PULSE(.5 1 0 .1u .1u 4.9u 10u)
SYMBOL res 448 32 R0
SYMATTR InstName RESR
SYMATTR Value .1
TEXT -144 -40 Left 0 !;op
TEXT -144 -16 Left 0 !;ac oct 100 100 1meg
TEXT -144 -64 Left 0 !.tran 0 20u 0
TEXT 96 -16 Left 0 !.options plotwinsize=0 |
|
|
| keantoken |
Wow, you must have magic fingers! It works great now...
:confused:
How? What does the 100-ohm resistor do?
- keantoken |
|
|
| sawreyrw |
keantoken,
Good question: What does the 100-ohm resistor do?
The answer is nothing useful and it could be deleted. Actually, the simulator had problems with a 2N2222 as Q2 and I was trying some things to overcome it. (It's a problem with the 2N2222 model.) Increasing the 100 ohm resistor would help, but again, the 2N2222 is at fault.
Rick |
|
|
|
