Another Power Supply

[Kleinstein]

For the simulation of the regulator you don't need to include the rectifier - the two parts are well separated and can be treated separately. This makes the simulation simpler and faster.

Instead of a Darlington transistor you can use two separate transistors. The choice of using a power transistor in DPAK is poor - this may OK for the first in a darlington configuration, but not to dump the main heat part. Consider at least a TO220 or better even TO247 that are much easier to mount to heat sink. SMD transistors would need cooling through the board and thus usually large GND planes or similar.

The usual OPs don't like driving lower than 50 Ohms load. The simulations might be overly optimistic i this respect, so one should have a resistor between the OP and the transistors. Even if relatively small this will influence the regulation.
Even if you just simulate the voltage loop, you should include the shunt used for current limiting, as this will influence the performance. At some places (e.g. emitter of the output transistor) it can actually help to stabilize the voltage regulation, but in other positions it can also make things more difficult.

You will find out, if a negative supply is needed or wanted. It could make the regulator easier or faster.

The regulator simulated above is very slow - so stability is still relatively easy.

Looking at the output impedance is one way to check for all load impedances. If the phase shift is within the +-90 degree band, the circuit will be stable with any passive (e.g. combination of RLC and DC current sink) load. If not you can see at which frequency and capacitance it can oscillate. The only thing to vary is the load current - e.g. test at high and low currents.
The aim should be something like a 0.5-5 Ohms maximum impedance, that is reached at about 50-500 kHz. At higher frequencies the output capacitor determines the impedance, going down to it's ESR.  Preferably the maximum in impedance is a little flat, not strongly peaked (with output capacitance only).  Towards lower frequencies impedance should go down no faster than proportional to frequency - a stepper curve tends to be unstable. So the regulator output will behave similar to a inductance in the 1-20 µH range.

To check behavior in time domain, using a variable set-point is of limited use. It is better to use a step in load current, e.g. a current source with pulse shape (e.g. 1 µs rise / fall, pulse of something like 10-50 ms, e.g. 1 A to 0.1 A).

[SteveP]

Man, good progress!

Couple of comments: Heat: that transistor has an Rtheta j-c of 2.78C/W. Times 40 watts is a 112C temp rise--assuming that *if* the case is kept at 20C (which it can't be), you're at 132C. The max junction temp spec is 150C; you want to run your devices quite a bit lower than that if you want them to last. I typically think of keeping mine to around 100C, though others may be willing to go higher. You will need to mount the pass device to some sort of heatsink: either PCB copper or (much more likely) a chunk of aluminum. The heatsink has a thermal resistance just like the device. You need to add that in to the calc to get the final junction temperature. A non fan-cooled smallish aluminum heat sink has an Rtheta of a few degrees/Watt so now your device can only dissipate half (or less) of your desired 40 Watts.

If you noticed in the first link I gave you there is a comment (near bottom of page 4) that NPN regulators are *unconditionally* stable (Yippee!), so your choice of an NPN device has helped you there. It would be a different story if you tried an N-Fet.

You've done some good testing. Here's the one you're missing: grab a "load" from the device list; define it by clicking on "advanced" in its dialog. Choose "pulse". The dialog will change and allow you to enter some values. "I1" is what the load starts drawing, so put in something like 0.1A; for the second (what it will draw as the pulse) put in something like 1.1A. Use something like .1 seconds for the delay, so you can see what the stable situation is, put in something like .001 seconds for rise and fall times, put in about .1 seconds for on time. Graph the output voltage; what you want to see is that the output voltage stays constant (or very very close to it). You shouldn't see spikes or huge dips just before or after the current changes. Now change the rise and fall times to one microsecond and repeat.

You will want something to compare against. Grab the data sheets for the LM117/317 and the LT3080. In the textual specs you'll see that the LM117/317 is spec'd for 0.1% for load regulation and that the 3080 is spec'd for 1mV. You'll want to be in that range. Then, look at the graphs for "load transient response" (there are also graphs for "*line* transient response"). At the bottom of the *load* transient graph is the change in current demand, the top of the graph is the vreg's response. Notice  how slow the pulse is for the LM117/317 leading/trailing edges-- almost 5uSec. That's because the LM117/317 is pretty poor and if they showed the response for faster edges it would look really really horrible. Compare the graph for the 3080--those leading edges are darned near vertical and the response is quite a bit better. You'll notice dips/spikes at the moment the current changes. Minimizing these is part of the challenge. (Notice that the LM317's response is measured in *volts* and the 3080 is measured in mV--quite the difference!)

Aside from accurate regulation and no spikes, you also want to look at "settle time"--how *fast* does the voltage settle to its ultimate value. This is often 10s of microseconds, although faster is entirely possible. Good commercial power supplies (e.g., HP/Agilent) try to settle to some small percentage within 25usec IIRC.

If you want to play some, make a little test circuit and try a pulse test with an LM317 and an LT3080 (they're both in LT's "Power" folder--the 317 is the LT317A). You'll see a big difference and you'll start to see where your circuit/components fit in. You can decide whether you want to be an LM317 (or worse) or an LT3080 or somewhere in between.

On another subject, the images you attach are really hard for me to read on my machine--kinda looks like you're using something other than LTSpice to do a screen capture and then attaching those?? What most folks seem to do is go under Tools and use "Copy bitmap to clipboard" which makes a high-quality bitmap, then attach that. [The bitmap it makes is from whatever window (plot or schematic) is active]

At this point, my suggestion would be to make sure your pass device/heat sink can really handle the heat (with room to spare). If you can find a way to make it work with the NPN BJT, you'll be ahead of the game. If you have to switch to a mosfet, now would be the time to do it--they get driven (from the op amp) in different ways and they affect the compensation network quite differently.

You're doing great!

--Steve

[Kleinstein]

Usually a lab power supply is not as fast in regulation as these simple regulator chips. The regulator chips are made to work with a reasonable well behaved load, while a lab power supply should work with essentially every possible load. This requires the lab supply to make some compromises that makes them slower. Also the usually very limited power rating of the integrated regulators allows them to use rather fast transistors. It gets really difficult to make a lab supply that fast - even if it works in the simulations, there are parasitic effects (e.g. inductance and inductive coupling) that makes it really hard.

A good guess to get it fast with an external power device, something like an LT1575 would be a choice. But this is not a simple things as layout is critical.

[SteveP]

Kleinstein: I do see what you're saying and I somewhat agree. However:

1) The point of this exercise, according to the OP's initial statement, was to *learn*. In my opinion you don't learn by making things really really slow--if you do, you never run into the tough issues in simulation, though you might when you start playing with actual components. I think it's better to hit the issues first in simulation where it's easier to see what's going on and to make changes. In simulation, in other words, you have to make things fast to learn what the issues are for the exact reason that the simulation doesn't (typically) include the parasitic effects you mention. Also, my suggestion was to compare a *simulated* LM317 against a *simulated* candidate design. Apples to apples.

2) To your point that bench supplies typically aren't as restricted in current/voltage as chip voltage regulators, in this case  the OPs design envelope (20v, 2A) puts it squarely within the envelope of the LT3083 and not far from the LM317 (2A vs 1.5A). I am not sure that I agree that chips are not meant to handle the variety of loads that bench supplies must face--the datasheet for the LT308x series doesn't seem to suggest there are any restrictions as long as the voltage, current, and temperature specs are met, though perhaps I missed something.

3) I suspect that even an old design like an HP 3610, 3611, 3612 would not be as bad as an LM317.

4) I ran sims of prasimix's power supply (the .asc files are publicly available). They simmed pretty darned well and it is my understanding that the hardware performs similarly. That may, however, fall under your category of it being "really hard"--he put a lot of work into those boards. 

5) At some point one moves from simulation to the real world. In my view, that's the stage in learning where one considers in detail the issues you mention, as well as others (like models of devices don't simulate accurately, etc.). Before then, when learning, you don't really have the background to appreciate the issues inherent in that step.

In short, I agree that there is a point to consider everything you mention. My belief is that the OP is not yet at that point.
--Steve

[Kleinstein]

Like most lab supplies the old HP3610 is very likely slower in response to load changes than a LM317 with a moderate load. The LM317 is actually quite fast. This can get different with a larger capacitance at the output. The regulator chip likely will not oscillate, but expect quite some ringing with a large low ESR cap.

So my point is, that there is no need to make the first regulator design that fast. If you get 1/10 the speed of a LM317 this could be still an acceptable lab supply - there are supplies that are even slower. There just is no need to get much faster than the commercial designs for the  first try. However the suggestion with a 1 µF integrating cap is to slow to be practical.  Just for learning it's not so bad to start very slow first to make the simulation run stable, check for DC values and only than adjust for higher speed.  The same also works for real parts.

For early designs it was a common way of adjustment to start slow first, check for DC performance, then make is faster until oscillating and than adjust back by a certain factor for the final setting.  This is somewhat similar to classic tuning of a PID controller by the Ziegler Nichols method.

[SteveP]

I think we are talking at cross purposes. You are talking about *designing a real thing* and I am talking about *learning*.

We do all sorts of things when we learn, so that we *can* learn. We assume that gravity is constant or that air has no effect on a falling object. We treat op amps as "ideal". Then, when we have the basics in our heads, we can consider more realistic conditions.

If you don't, at some point, push the bounds of the envelope, you never learn that there *is* an envelope and you never know where those bounds are. I didn't learn very much about regulation until I fought with oscillation. If you never create a circuit which oscillates, how will you ever learn about it? I agree that you want to get to a point where it does *not* oscillate, but my point is that when learning about regulation you *do* have to fight that battle, and that a good way to create that battle is to try to make something fast.

The OP has already created a circuit that is stable. I think it is now time for him to learn about oscillation. Of course, that's his choice, but I think it's an absolutely necessary part of learning about power supplies.

In fact, one way to look at the essence of regulation is to see it as a balancing act between speed, accuracy, and stability (as well as the usual other issues). In my opinion, until you've dealt with that balancing act, you haven't really learned the deeper issues of regulation.

--Steve

P.S. To Brad: I feel totally weird talking about you behind your back like this; hope you don't mind the meta discussion :-)

[braddrew0]

Not at all, I appreciate both of you taking the time to help me. And you both have valid points - this design is a learn-what-I-don't-know type, but I do want an understanding of how something more complex works for future designs. I'm trying to absorb as much of what you both say as I can - a lot times I have an idea of where I want to go but not how to get there. The detail you're both providing is great

There's a lot of information in your last posts (and I can't believe I spent so long trying to add a variable load without adding a load that's variable....  ). It's going to take me a few days to absorb it all and run my next tests. In the meantime, I want to briefly touch on the cooling side.

What I've tried to do with my designs is add in things which will work, but aren't recommended. A lot of recommendations here are subjective - not to take away the fact that they're based on considerable levels of experience which I don't have - my goal is to gain that experience by trying things that aren't necessarily the "right" way. As an example, my last design I decided to use 0603 components for all of the resistors, caps and LEDs. I didn't have a space requirement (in fact the board was bigger than if I used through hole - I wanted room to solder ) but I wanted an appreciation of the hassle associated with using them, so next time I come up with an idea that "requires" 0603 I'll have an appreciation of how hard that is to do and whether it's worth it. And I learnt that all the advice on here is absolutely correct, 0603 is a pain to solder! It's not a case of being difficult, it's just really fiddly with pieces sticking to the soldering iron and half a dozen 0.1uF ceramics that are probably in the vacuum cleaner by now... regardless, I now know what the cost is of using 0603 and I'll think harder before I use them.

So in a similar way, one of my objectives here was to use an SMD pass through device. And I totally get that it's not recommended and cooling will be a major issue. I have a couple of designs in mind for later where I'm not going to have a real choice on SMD or not, so I wanted to use this as an excuse to learn about properly cooling SMD (hence why I already had an answer for you when you asked about cooling before - it's definitely forefront in my mind ).

So saying that, I thought about a better way to attack this today and I'm leaning toward a software current limit. I originally came up with 2A based on a 5V 2A charger - enough to implement a charging circuit one day if the design is suitable. I don't have any requirement to hit 20V @ 2A - I think I will use 20V and I think I will use 2A but not both at the same time (at least not in the near future - and now I'm learning how to make something that will exceed that ).

So what I'm thinking is a software current limit to a max of 2A @ 10V, linearly decreasing to 1A @ 20V. That gives me a maximum of 20W of power. I don't anticipate that I'll operate it to these limits, but I want it to obviously be safe to do so. I'm still planning to use both a cooling ground plane and a surface mount heatsink. So by the datasheets, I have:

Rtheta-JC = 2.78 deg/W
Rtheta-JA = 71.74 deg/W
Heatsink Thermal Resistance = 15 deg/W
Tmax - 150 deg C

Does this mean that this device will run at approx 1500 degrees above ambient at 20W? How do I take into account the effect of the heatsink? I can't wrap my head around how 10W of power dissipated on one device will correlate to the same cooling effect as 10W of power dissipation on a different device, if they're both made out of different materials?

Is there any way to make the SMD device work with these limitations?

Thanks again guys, really appreciate the help

[mij59]

The thermal resistance Rtheta-JA = junction to air, so without the use of a heat sink, check the data sheet how this defined.
The overall thermal resistance has to be much lower,  even with a total thermal resistance 17.78 C/W the temperature rise will be 355 C @ 20 W

[braddrew0]

OK, that makes sense - so rough numbers realistically you wouldn't want to pass more than about 3W... even with forced air (brings it down to 11 deg/W) you'd probably want to limit to 4-5W. With a D2PAK the non-forced case is around 11 deg/W so same limit, but if you force air through it (600 LFM) that drops to 3 deg/W... I'd say 20W would be technically achievable here provided you found a D2PAK with similar theta jc and you included a decent sized fan, but that's probably pushing the limits of what I wanted to do here - I guess that means I'll be switching to through hole... 

Thanks again for the help

[Kleinstein]

Calculating the efficiency of heat sinks is a little tricky. In first approximations there is a heat resistance rather similar the electrical resistance. However the transfer from the heat sink to air depends on the conditions, like air flow, orientation and surrounding. Also heat can drive there own convection flow - this makes thermal resistance nonlinear. There are approximate formulas on how effective cooling through the board is. This may work for 2 or 4 W but not really good at 20 W. If you want, one can solder a TO220 like a SMT part.

As a rule of thumb it is a good idea to use only about half (maybe 2/3) of the P_tot rating of power transistors. This makes cooling easier, as the case can then be at up to about 80 C as opposed to 25 C for the full P_tot rating. With a reasonable heat sink the temperature should be below 60 C, so you avoid burns form touch. Transistors are not that expensive any more, so it can be worth using a larger transistor instead of a larger heat sink.

Current liming usually should be fast, as one purpose is to protect the circuit and the supply. So a software only solution is not that great and would need at least a fast backup to protect the regulator.

For a linear supply using a single transformer tap, the maximum heat loss occurs at a short with maximum current. The power will be raw voltage times current. So for a 20 V 2 A supply this could be up to about 50 W (assuming about 25 V raw voltage) - reducing the current limit at high voltage does not change anything. If at all the opposite helps, this is called foldback current limiting - the maximum current gets smaller at low voltages. Many chip regulators like the LM317 use foldback, but lab supplies usually not, as this may cause instabilities with some loads.

Its a different thing if a second transformer tap is used - this reduces the maximum power loss, except for short transients. At low power like here using a second tap is not very common. 50W  is still easy to cope with, with a single transistor like 2N3055.

[braddrew0]

This cooling thing is still getting me - even if I keep below around 3 deg/W total thermal resistance, under normal max conditions that would be a temp rise of 120 deg (giving 30 degrees ambient max, assuming I'm happy to let it get damaged at 30.1 ambient). But to even get to 3W unforced, I need less than around 2 deg/W thermal resistance on the heatsink. Digikey (http://www.digikey.com/product-search/en/fans-thermal-management/thermal-heat-sinks/1179752?FV=fff40012%2Cfff80068%2Ce68004c%2Ce68004d%2Ce680053%2Ce68006c%2Ce68006d%2Ce6800c6%2Ce6800c7%2Ce6800cc%2Ce6800d0%2Ce6800d2%2Ce6800d3%2Ce6800d4%2Ce6800d6%2Ce6800d7%2Ce6800d8%2Ce6800da%2Ce6800db%2Ce6800dd%2Ce6800de%2Ce6800df%2Ce6800e0%2Ce6800e1%2Ce6800e2%2Ce6800ea%2Ce6800f4%2Ce6800f5%2Ce6800f6%2Ce6800f7%2Ce6800f8%2Ce6800f9%2Ce6800fa&mnonly=0&newproducts=0&ColumnSort=1000011&page=1&stock=1&pbfree=0&rohs=0&k=&quantity=&ptm=0&fid=0&pageSize=25) gives me a bunch of options, but they start at around $15 and go up pretty quickly from there...

So I guess this is what you were talking about Steve, with a BJT 40W isn't really achievable without forced air? Are there any other tricks to employ here?

[braddrew0]

Sorry should clarify - any tricks that don't involve forced air or paralleling transistors?

[mij59]

Sorry should clarify - any tricks that don't involve forced air or paralleling transistors?

Paralleling transistors makes no difference, you’ll need a preregulator.

[SteveP]

He he, welcome to power supply design :-)

Big picture comment: to design a power supply means juggling heat, voltage, current, stability, accuracy, speed, sometimes cost, and functionality, among other things. It's a lot to juggle.

I get that you like to push the envelope. That's great! One of the great things about at least *investigating* something others don't usually do is that you will find out why they don't do it. Then, if you are lucky, you'll think outside the box and come up with something others haven't thought of. I think that's called "progress" :-) If you are not so lucky, you'll have to relax a constraint or two, but at least you'll know *why* you're doing so. You will also gain a real appreciation for just how great some of the designs you'll see really are (and how crappy some others are).

In dealing with heat, there are the usual suspects:

1) paralleling devices *does* work--there are lots of commercial PSUs that have paralleled a few devices; the HP 36xx series I mentioned earlier paralleled four pass devices. (I mention that series because the schematics are available online.) You still need a (usually big) heat sink, but it spreads the load across more heat sink area and each device (obviously) needs to dissipate less heat. The issue with paralleling devices is that you need to take steps to get them to share the current equally; the resistance of some devices (BJTs) drops as they warm up, so they pass more current which heats them up more, and you get thermal runaway. If you try to parallel them, one will inevitably carry a bit more current than the others, so it heats up more, starting the thermal runaway scenario. Mosfets typically *raise* their resistance as they heat up, so you don't tend to get thermal runaway. There are techniques for dealing with BJTs in parallel, but that's outside my area of knowledge, so you'd have to research that one on your own. Mosfets are paralleled all the time--for example, the controllers for electric vehicles (many KW) have been doing it for years.

2) You can switch to a pass device with a lower Rtheta. Rtheta isn't a searchable characteristic on websites like Digikey, but you can use Power as a surrogate. Mosfets typically have a lower Rtheta, sometimes *very low* (.05 W/C is the lowest I've seen). I don't recall what the lowest Rtheta is for BJTs. The 3055 (but not SMD) mentioned by K is about 1.52 W/C in the TO-3 case and the datasheet claims you can run it at 200C, just to give you a reference point ( was looking at the one from ON-Semiconductor).

3) There are pre-regulators and there are pre-regulators. I agree wholeheartedly with the decision to not tackle a "real" pre-regulator for now, but you can use a simple one:  the "high low" switch. Transformers today typically do not have a bunch of taps like they did in "the old days". However, many transformers *do* come with one "tap"--the outputs can be put in series or parallel. Use a DPDT switch to switch the transformer leads from series to parallel when you want low voltage--it will cut the drop across the pass device(s) by half which cuts the power dissipation by the same amount.

4) Don't know if you've gone down this path yet, but you can stitch together (with vias)  top side and bottom side PCB copper to get increased dissipation. I've never gone that route, but lots of designs for other things do, so the info is likely out there regarding Rtheta of that construction. I suspect it wouldn't be sufficient for 40W, however. You could also try to solder some small copper "fins" to the SMD's pad to decrease Rtheta.

5) You could solder an SMD pass device to a sheet of copper and get a lower Rtheta for that vs. what you'll get on a PCB, but I doubt you'd get as low as you need to and it probably defeats the whole reason you're considering SMD in the first place. Just to continue the thought, however, soldering to copper sheets is done with lighting LEDs all the time. There are online calculators for *simple* (flat plate) heat sinks. You can also search Digikey for heatsinks to get a *rough* idea of how much heat can be dissipated by the various types, but the Mfrs often use extremely optimistic numbers; I'm not a passive heatsink guru (though I've done my share of heat calcs for solid bars of various materials) but I'd suggest cutting them by half. The idea here being that you'd make a copper heatsink like an aluminum one; you'd use the Rtheta of the commercial aluminum one to guide your design of the copper one. You can also use the flat plate of copper as a heat "spreader" and fasten that to a larger aluminum heat sink.  In the end, you'd probably have to do a prototype of just the transistor and see how hot it really gets. The bottom line, of course, is that PCB copper can only dissipate a certain amount of heat--period.

5) forced air; yeah, I know :-(  But it really gets rid of a lot of heat....

Of course, you can use a combination of the above. Sometimes that can get you where you need to go without making too many sacrifices. E.g., a high-low switch and a different pass device. Or you find a pass device with a higher junction temperature rating. And/or you decide to run right at the junction temp rating (*not* recommended for a whole bunch of reasons).

You may find yourself making some unpalatable design decisions here....as I said at the outset, I went back and forth on pass devices many times before I settled on one. Part of it was heat--mosfets were great for heat, terrible for stability. BTJs the opposite. When I thought I had heat licked using mosfets, I fought instability until I went nuts. Then I went back to BJT and fought with heat until I went nuts. I looked at *a lot* of data sheets :-)

--Steve

Edit: corrected Rtheta j-c for 3055 due to misreading the datasheet....

[Kleinstein]

With just 40 or 50 W it is possibly to use a single BJT or suitable MOSFETs. You just need to choose one that is powerful enough and has a low internal thermal resistance. Something like a 2N3055 (TO3 case) or TIP3055 ( To218) will do it. With a smaller transistor you need a larger heatsink.

Paralleling BJTs is relatively easy, with just resistors at the emitter. Paralleling MOSFETs works well in a switching application but is more difficult in a linear application like the linear regulator. Here resistors at the source pins are needed which usually need to be larger than with BJTs. In addition the MOSFETs need to be matched.

[braddrew0]

And it just clicked on the drive into work this morning that I'm making the same mistake I made before with the 7805 temp calculation - I've been looking at power through the transistor = heat where I should have been looking at power dropped = heat... That means I really need to pass 34V * 2A = 68W....  It means a lot of your comments make more sense now, like why low voltage high current is the worst case...

Kleinstein, I did look at that one - unless my maths is wrong, I couldn't cool it to a reasonable temp even with 40W? I get theta jc as 1.52, so 40W = 60.8 above ambient, but then the heatsink kills me - the first <$10 heatsink for TO-3 has a thermal resistance of 5 deg/W (http://www.digikey.com/product-detail/en/500403B00000G/HS264-ND/373756), so that would add 200 deg on it's own, giving ambient + ~260deg at max power?

Even going top of the line at $156 for the heatsink (http://www.digikey.com/product-detail/en/HS04/598-1472-ND/1762106) it has  thermal resistance of 0.95 deg/W - so my 68W would sit at 170 degrees above ambient... ouch! 

I'm starting to lean towards paralleling the output to increase the current. That means I can drop down to something cheaper like a 2N6045 (http://www.digikey.com/product-detail/en/2N6045G/2N6045GOS-ND/918259) with a reasonable heatsink (http://www.digikey.com/product-detail/en/530002B02500G/HS380-ND/1216384). That's about $2.50 per couple and if I split the 68W over 4 I get a max temp of about 73 above ambient on each - so with 30 ambient that gives me about 50 degrees flex in case one of the devices heats faster than the others?

And I will address all the points you've all made - I've read them all, just trying to process some of it. Thanks again for the help

[mij59]

When sourcing components check several vendors.

For heat sinks you use something like this http://www.reichelt.de/Luefteraggregate/LAM-3100-12V/3/index.html?&ACTION=3&LA=2&ARTICLE=75424&GROUPID=3751&artnr=LAM+3100+12V  .
You'll need some airflow in the enclosure anyway.

[braddrew0]

Thanks mij59 - I think I'm going caseless for this one but I've bookmarked the site for future reference

On another topic, if I parallel the BJTs, do I need to use resistors on each of the emitters?

[mij59]

Thanks mij59 - I think I'm going caseless for this one but I've bookmarked the site for future reference

On another topic, if I parallel the BJTs, do I need to use resistors on each of the emitters?

If the transistors are exactly the same no, but they are kind a hard to find in the wild.

[SteveP]

Wait, why is it 34 volts? Last I saw it was 20v. If you want an output voltage of .001 volts, you'd drop about 20v * 2A = 40 watts. What am I missing?
--Steve

[braddrew0]

Steve my initial input was 18VAC which I could smooth to the range 26-25V using 40,000uF of input capacitance. I changed that to 24VAC in with 4,700uF which gives me 34-28V (both assuming 2.5A draw which is 2A + "some" for regulator, uC, overswing, etc). So my max input is 34V and max drop would be 34V @ 2A = 68W (although this obviously isn't constant).

My original plan called for 24V @ 2A max (hence 26-25V) but I got rid of that early because I wanted to cap the power at 40W. Now I can see the high end doesn't really matter (except pass device drop) so I may bring that back in.

[braddrew0]

And sorry, one more random thought on that power calculation - at low current draw there would be minimal ripple, which means at (for example) 0.001V and 0.001A the pass device would be generating a solid 68W of heat.

[SteveP]

OK, got it, thanks. I just plain missed the part where you earlier explained about the ripple. Yeah, 68 watts is harder than 40 :-)

While you're thinking about heat, here are a couple of more things you may want to consider...

1. Once you get the heat out of the device and into the heatsink, you need to (obviously) get it from the heatsink to the air. But where is the air? You probably don't want it *inside* the enclosure (I know, for this first version there isn't an enclosure, but *someday* there probably will be so you might as well think about it a little now...) for a couple of reasons:
  a) you don't want to bake your other components. Yeah, you'll have the usual plethora of ventilation holes, but the air inside will still be hotter than outside.
  b) you want the coolest air possible hitting your heatsink because what matters is the difference in temperature between the heatsink and the surrounding air.

So you'll probably want a design/devices that allow at least a portion, if not all of, the heatsink to be outside the enclosure.

2. You may or may not have noticed, but the part of your pass device that attaches to the heatsink is *live*. That makes the heatsink live and if the heatsink is outside the enclosure, you may not want the heatsink to be live. This means you'll need an electrically insulating material between the device and the heatsink. Problem, is, those are also *thermally* insulating which means there's one more bit of thermal resistance you have to account for. If you search places like Digikey for "thermal pad" you'll find what you're looking for. In the TO-220 size, they seem to range from about 0.35C/W up to about 0.75C/W. Doesn't seem like a lot until you multiply it by the 68 Watts. This will tend to drive the cost of your heat sink up, since it has to be more efficient (i.e., bigger).

If you haven't figured this out, heat is a major driver of linear power supply design :-)
--Steve

[braddrew0]

To be fair, heat only started becoming an issue when I started doing the calculations correctly... 

Good points Steve - I knew about the thermal pads but didn't consider you'd have to take them into account, so that's a good learning point. I remember about 20 years ago from building computers in my teens that CPU heatsinks work significantly better with good quality thermal paste - that's one thing I was planning to do, although I assume the manufacturers figures are based on the best case scenario, so that's probably only stopping any more loss. I think the next design (and anything in an enclosure) will definitely be based on a switching pre-reg - I do want to get this one built simply though, just to show myself that what looks good on paper actually works (or doesn't....)

So with that, I think I have a plan. I think I'll switch back to 18VAC in, with the 40,000uF filters. If my math is correct, that's 25.46-24.83V @ 2.5A. If I use two NTP5864N N Channel MOSFETs (http://www.onsemi.com/pub_link/Collateral/NTP5864N-D.PDF) with the Aavid non-forced heatsink from before (http://www.digikey.com/product-detail/en/530002B02500G/HS380-ND/1216384) that's a total thermal resistance of 4deg / W. So each device would need to drop a maximum ~26W, which is 104 deg. This is hot, but still workable in a normal (up to 30 deg) ambient environment. As a bonus, the two MOSFETS will naturally equalise current so I'm not as worried about one getting hotter than the other (like I was before). I should mention as well that the NTP5864N is good to 175 deg

For bonus points as well - the data sheet specifies a max Rds of 12.4 mohm. With a 100 mohm pass resistor, then at 2A I could expect a ~225mV voltage drop, which means I can (maybe) regulate to 24V! 

[Kleinstein]

Using two small MOSFETs in parallel is a poor decision: They would need rather large source resistors (e.g. 0.5-1 Ohms)
to make them share the load. Thus the voltage drop will be rather large. At 2 A and 25 V raw supply you could get away with just one larger MOSFET (e.g. IRFP240) or BJT.

Using MOSFETs also needs something like 3 V higher voltage to drive the gate.