Saving a Heathkit IP-20 0-50VDC, 1.5A power supply - Page 1
Forum section: electronics / projects

author: MisterHeadache
author_rank: Regular Contributor
timestamp: June 05, 2025, 02:50:45 pm
content: I picked up a Heathkit IP-20 for $10 at Hamvention this year. It's bones are in OK shape but the regulator circuit has been heavily hacked up and it is not functional. Rather than repair it (it uses a handful of rare/expensive germanium PNP transistors), I want to remodel the circuit to use modern bits and pieces. I think it'll make a great project!I'm taking a different approach with this one, mainly because I've never designed a current limiting adjustable voltage linear power supply. I'm fresh off of watching Dave's video series on the microsupply, so that got me started. But rather than sweat for weeks over detailed circuits and sims, I decided instead to start more abstract and first put together a block diagram of my ideas and crowd-source it for critique. So that's what I've done - see the attached image.QUESTIONS: Will this work? Am I missing any big items on the block diagram? If I'm on the right track, I'll proceed next to drawing up the detailed circuit for further analysis.For reference, here are the original IP-20 specifications, which I would like to still meet (or even exceed where practical)Output: 0.5-50V, 1.5A maxLoad regulation: +/-15mVLine regulation (105-125VAC): <0.005% changeRipple and noise: 150uV maxTransient response: <25usCoarse Voltage adjustment settings: 5, 10, 15, 20, 25, 30, 35, 40, 45, and 50VFine Voltage adjustment settings: +0V/-6V variable from the coarse setting (example: at 25V coarse setting you can fine adjust from 19-25V)Coarse Current limit settings: 50mA, 150mA, 500mA, and 1.5AFine Current limit: 30% to 110% of the coarse settingMajor parts that I'm keeping are the transformer and all the front panel controls, switches, and meter (with the exception of the fine voltage and fine current controls - they likely will need to be new value potentiometers).Thoughts:Existing design wastes A LOT of power as heat in the regulation circuit! 12 Watts at max (1.5A) current on 5V setting, increases up to 36 Watts at max current on 50V setting, assuming no sag in E2 voltage. With the LT3083 I can do much better (example: I certainly don't need to feed it 74V to get 50V regulated output.) So I may want to reassign the secondary taps down 1-2 places.I'm targeting using a 2N3055 (plus other popcorn parts) to build the current limiter because I've got a stash of those power transistors and wanna use them in something.Transient voltages when switching voltage ranges. This actually caused damage to transistors in the IP-27, the successor to the IP-20 that used a very similar circuit. Apparently Heathkit issued a service kit to fix it. How do I prevent damage during range changes?The LT3083 has to be floating, it cannot withstand 74VDC across it, so I'll have to be careful to isolate it. Which is why I'm using the FET ahead of it and the Zener across it like as shown on page 19 of the data sheet.I'm trying to stay away from op amps because I'd need ones that can withstand at least 74V (that's the highest no-load voltage on the transformer secondary). High voltage op amps are expensive (example: the OPA454, a 100V rated part, is $7 per amplifier) and I'd need several of them to mimic Dave's microsupply architecture.The easiest and likely cheapest solution would be to chuck the IP-20 into the recycle bin and buy a modern supply - but where's the fun in that??

author: Doctorandus_P
author_rank: Super Contributor
timestamp: June 05, 2025, 06:04:52 pm
content: I'm guessing LT3083 is relatively expensive, much more so then a 2n3055.50V is also quite high (have not checked on the limits of a 2n3055. The bog standard BJT these days is 2SC5200. It's TO247, does 200V 10A 150W or thereabouts.30Watt heat dissipation is not very much for a lab power supply. These things are usually not built for power efficiency. If you really want more power efficiency, the first thing to do is to add some relays, that switch transformer coils depending on the required output voltage.There are some vintage power supplies that use thyristors in the AC part right after the transformer.A more modern approach is to add a switching pre-regulator.I don't know what your experience level with elecronics is, but if you're past the total beginner stage, then designing and building your own lab power supply from discrete parts can be a fun and educational challenge. There are plenty of example schematics and design documents on the 'web.Although if you go this way. I recommend you start with more modest specifications. Something like 20V 1A.

author: MisterHeadache
author_rank: Regular Contributor
timestamp: June 06, 2025, 12:48:52 am
content: Quote from: Doctorandus_P on June 05, 2025, 06:04:52 pmLT3083 goes for about $12 each2N3055 is 60V so it is marginal. I'll look at the 2SC5200There is already a rotary switch used to select the various secondary taps, I plan to retain itYeah, I know there's better ways, but I want to take at stab at making this guy useful again. If covering the full voltage range turns out to be too much time/$$$, then I'll look at reducing it.

author: MathWizard
author_rank: Super Contributor
timestamp: June 07, 2025, 07:21:44 am
content: You can always add another small transformer, and make some low voltage supply rails, and tie their GND to the positive O/P terminal, at lot of supplies to that. Depending on where you live, it shouldn't be that hard to salvage a little transformer or 2, like out of old stereo's, wall plugs, alarm clocks, microwave ovens, etc.Here's the output drive on a 30V-3A channel, with 2x 2N3055, they get up to over 45W each. The +/-24V and +/-15V rails have their GND on the +OP. The main power rail is maybe 35-50V, I haven't checked it yet.The rotary switches give me an idea for that PSU below, I could add some wires and a switch, so I could unplug the PSU's voltage or current pot's, and plug them into my resistor box.

author: Hydron
author_rank: Super Contributor
timestamp: June 07, 2025, 08:32:35 am
content: I think the original uses foldback current limiting as it cannot handle the dissipation required for a constant current mode (this is why it also has so many ranges). I'd second the suggestion to add range switching relays - that would let you make it operate more like a modern supply and avoid crazy power dissipation.I've actually got a working one in a box complete with original manual, however said box is on the other side of the world!

author: MisterHeadache
author_rank: Regular Contributor
timestamp: June 09, 2025, 07:03:30 pm
content: Quote from: Hydron on June 07, 2025, 08:32:35 amHmm...the manual seems to indicate it's just limiting current, not foldback limiting. Nonetheless, I'm gonna study it a bit further and may even build a simple simulation using a generic Germanium PNP transistor model just to satisfy my curiosity.Also, maybe I am mis-understanding the suggestion about the switching relays because there already is manual switching in 5V increments. Or are you suggesting to automate the selection of the appropriate secondary tap?

author: MisterHeadache
author_rank: Regular Contributor
timestamp: June 17, 2025, 01:39:49 pm
content: Here’s my first-pass circuit design for this project. I’ve taken some key elements from Dave’s uSupply project where I could. Looking for your constructive feedback please! This isn’t a complete circuit yet, among other things there’s no fixed current load on the regulator output yet.Keeping in mind the original specs that I stated on the starter post, here’s some key design details:“VDC UNREG” comes from the existing IP-20 transformer and a basic bridge rectifier/capacitor filter. It is user selectable in ten different ranges from 14VDC to 74VDC.“Vref” comes from the existing ‘precision’ reference voltage circuit on the IP-20 and ranges from 5V to 50V, corresponding to the same user selected control that selects “VDC UNREG”. It feeds into the SET pin on the LT3083. The rest of the circuit around the LT3083 comes right off the application data sheet for use at voltages above the 18V max rating.The INA281A1/B1 with a 200 mOhm sense resistor outputs 4V/A. It can handle 110V max common mode voltages while being driven by a much lower supply (12V in my case). 4V/A works acceptably for scaling the lowest current (50mA equals 200mV) and highest current (1.5A equals 6V). The output of the INA281 feeds into the non-inverting input of an LM358.The inverting input of the LM358 is connected to a reference voltage that corresponds to the user selected maximum current limit. It comes from a simple resistor voltage divider configured to give the reference voltages that correspond to 50mA (200mV), 150mA (600mV), 500mA (2V), and 1.5A (6V). Potentiometer RV1 provides the same 30% to 110% adjustment as a stock IP-20. Resistor Rt is different for each of the four current ranges, I will reconfigure the coarse current rotary control “CR” on the IP-20 schematic to select the appropriate value (75k, 22k, 6.2k or 1.1k).The LM358 output goes to transistor Q2. A 2N3904 won’t work here, it’s only rated to 40V and my Vref will be as high as 50V. It pulls to ground the SET if there is a current overload.I’ve run a first-pass simulation and this seems to work, but there’s a lot more that I need to stress it under, not the least of which is the power dissipation of the LT3083 and the BUZ11. I already see the need to parallel 2-3 of the BUZ11’s to keep from burning up things.I’m open to comments and suggestions.

author: MisterHeadache
author_rank: Regular Contributor
timestamp: June 29, 2025, 04:15:56 pm
content: OK, I've settled on the design shown in the attachment. There's still many details I need to fix, but I've got it working pretty well in my LTSpice simulations to yield what I want.One issue - the feedback loop between the current measurement made by the INA281, the LM358 reacting when the current exceeds the limit set by SW1 and then turning on Q2, which pulls down the LM317 set point and causes the current to drop. Once it drops below the SW1 set point, the LM358 turns off Q2 and the voltage starts going back up. All this happens at very high speed and oscillates rapidly, it is clearly not a stable control loop. However, by brute force I determined that adding 1-10uF of capacitance (C11) on Q2's base slows down the response and makes it a lot more stable.I'd like to do a proper phase margin study on this design in LTSpice, and I've watched a few tutorials and grasp the basics about what phase margin is. I see how to set up a study for a basic op amp feedback circuit, but how should I set it up for this circuit? As an ME I had to take control systems theory in undergrad but it never sunk in past the basics. Looking for a bit of help please.

author: MariuszD
author_rank: Regular Contributor
timestamp: July 06, 2025, 06:01:16 am
content: Do you have a working Ltspice simulation? Post it.Add AC source in series with U1 output.

author: NiHaoMike
author_rank: Super Contributor
timestamp: July 06, 2025, 01:24:10 pm
content: Do you actually need it to be low noise? Maybe consider using a buck converter instead.

author: MisterHeadache
author_rank: Regular Contributor
timestamp: July 08, 2025, 03:09:21 am
content: OK, my attempt at simulating gain margin is attached. Getting goofy looking results, so highly likely I'm doing something wrong here.Error log contains these concerning statements:Direct Newton iteration failed to find .op point.Gmin stepping failedSource stepping failedPseudo Transient succeeded in finding the operating point at 1.87957 s.Odd thing is, the same circuit in a transient simulation with R12 (the load resistor) slowly decreasing with time shows correct current clamping behavior with just a tiny bit of ringing.Quote from: NiHaoMike on July 06, 2025, 01:24:10 pmYeah, I want to stick with a linear design here.

author: MariuszD
author_rank: Regular Contributor
timestamp: July 09, 2025, 06:54:49 am
content: I don't have included models. Can you post it?

author: MisterHeadache
author_rank: Regular Contributor
timestamp: July 10, 2025, 02:16:52 am
content: Sorry, that would be helpfulI cannot attach .lib files, so I just renamed them to .txt files.

author: MariuszD
author_rank: Regular Contributor
timestamp: July 10, 2025, 07:41:39 am
content: Ina281a1 doesn't work properly.Before you posted the models i tried with generic parts. The circuit contained many phase delay circuits. I have no way to fix so many problems at once. I did it differently, I connected the amplifier and the transistor in one feedback loop, it's not a good solution because low phase marin in this inner loop, but it works in the simulation.There are other problems with this circiut. LT1086 cannot work with 57V input. Current limit circuit doesn't work below 1,3V.The LT1086 with a 100 nF output capacitor gives peaking at 2 MHz; the gain margin at this point is low. In transient simulation it oscillates anyway. With recommended 22 uF and added ESR 300 mOhm it works.

author: MisterHeadache
author_rank: Regular Contributor
timestamp: July 10, 2025, 11:46:11 pm
content: Quote from: MariuszD on July 10, 2025, 07:41:39 amThanks for the feedback! Interesting. The INA281A1 model does work correctly for 'slow' speed stuff. I've got a different simulation where I change the load resistance slowly over 1s and the INA281A1 reports the correct gain (3V per amp flowing through the 150mohm shunt).Regarding the LT1086 - I'm really gonna use an LM317HV, which is good to 60V, but I could not find a spice model of it. Otherwise I would've used it. Yep, I know the current limit drops off below 1.3V, its an imperfection that I'm tolerating for now. I'll play around with my sim based on what you've found.

author: MariuszD
author_rank: Regular Contributor
timestamp: July 11, 2025, 01:21:37 pm
content: Different approach: low-side current sensing. R5 is the current sense resistor.

author: MisterHeadache
author_rank: Regular Contributor
timestamp: July 17, 2025, 03:11:55 am
content: Quote from: MariuszD on July 11, 2025, 01:21:37 pmOK I built this in LTSpice and played around with it and I think I get it. When R12 is large, the voltage drop across R5 is lower than the current set point voltage, controlled by V2, so the output of U4 stays at/near the high rail. Thus preventing Q1 from conducting. However, as you decrease R12 to the point where the current going through it and R5 causes the voltage drop across R5 to exceed V2, U4 output now goes low, sinking the emitter current from Q1 and turning it on. U1's output continues to sink more current until the control loop reaches equilibrium at the op amp inputs.The ac sim that I ran very closely matches your image - phase margin is smack on 90 degrees.I'm gonna update my design to use this approach. Thanks!

author: ledtester
author_rank: Super Contributor
timestamp: July 17, 2025, 04:26:11 am
content: I hope the OP doesn't mind, but here is the first of the retrofit videos for anyone who's interested:Heathkit IP-20 Power Supply: Part #1 -- Level UP EE Labhttps://youtu.be/8-kT8BbtWtU

author: MisterHeadache
author_rank: Regular Contributor
timestamp: July 17, 2025, 04:00:05 pm
content: A new glitch - when I replace the generic OpAmp model for U4 for the LM358 model, the circuit no longer works. Looking deeper it seems that the op amp is unable to pull the emitter of Q1 low enough to ground to turn it on. Which is strange, the specs for the '358 say it can sink current, and that it can pull the output down to 20mV max above ground.I'm using the official Spice model for the '358 and I've used it in other sims before without trouble, so this is a head scratcher at the moment.

author: MariuszD
author_rank: Regular Contributor
timestamp: July 17, 2025, 04:17:26 pm
content: I forgot about this, for a current of 10mA the voltage drop across LM358 output stage is over 1V.You have unused 7VAC you can add negative supply voltage to get output of the LM358 <-1,3V

author: MisterHeadache
author_rank: Regular Contributor
timestamp: July 17, 2025, 09:02:10 pm
content: No worries, I was also falling into that trap for young players, as Dave often says.I'm already planning to use that 7VAC tap to make the +DC supply for the op amp and other circuits. As an alternative, I looked into op amp options that can get much closer to the negative rail at that current. The OPA310 for example can, while still preserving what looks like all the other props that I need. I can then use a LM7705 low noise negative bias charge pump to make a -0.23V rail for the OPA310. The LM7705 can sink upwards of 20mA, so that should be enough to handle the current coming out of the Q1 emitter.I'll update my sim tonight using those components and see how it goes.

author: MisterHeadache
author_rank: Regular Contributor
timestamp: July 18, 2025, 03:06:45 am
content: One step forward, two steps back. The sims worked great for phase margin but...the regulator won't regulate with low side current sensingEven a miliohm of R5 resistance causes the regulator output voltage to drop significantly with current. R3 needs to connect to ground to get the regulator to work, but then that causes the regulated voltage to drop across the output terminals as R5 voltage drop increases.

author: MariuszD
author_rank: Regular Contributor
timestamp: July 18, 2025, 12:10:34 pm
content: Quote from: MisterHeadache on July 18, 2025, 03:06:45 amWhy do you think that? R5 is outside the feedback loop.

author: MisterHeadache
author_rank: Regular Contributor
timestamp: July 18, 2025, 01:24:09 pm
content: With R5 out of the feedback loop it makes sense to me that the regulator should work fine, and hold steady voltage as the load R12 changes, but it doesn't in a 1s .tran simulation. The output voltage of the regulator is way too low by several volts. However, if all I do is make the change shown in the image, the regulator output voltage is spot on correct, but the voltage at the load is now lower, and of course drops further as the load increases and draws more current.It's quite possible I've made some other error in my sim, I won't be able to troubleshoot it further until tonight.

author: MisterHeadache
author_rank: Regular Contributor
timestamp: July 18, 2025, 10:47:51 pm
content: Found the problem and it was mei jacked up the input voltage at the LT1086 too high and that caused the issue. You did warn me, I just forgot about it when making a bunch of tweaks late last night.

author: MisterHeadache
author_rank: Regular Contributor
timestamp: July 19, 2025, 03:15:58 am
content: All right, here's my latest. OPA310 in place of the LM358, with a -0.23V supply to the negative power terminal (to simulate using a LM7705). For this phase margin sim, it doesn't matter if I use it or just connect the negative power terminal to GND, but on my transient sims it is needed. Anyway, the sim results in a phase margin of 80 degrees, gain margin of 42dB.A quick transient sim also shows great results. So now I'm into just tweaking things a bit and pulling together the circuit schematic in KiCAD (will post it later).

author: MariuszD
author_rank: Regular Contributor
timestamp: July 19, 2025, 09:24:30 am
content: I tested the current limiting circuit simulation with different currents, different output capacitors, and different regulators (LM317, RH117, LT1086). Many times I observed instability caused by the voltage regulator itself. The spice model LM317 from TI is very prone to oscillations, LT1086 is somewhat better in this regard, and RH117 causes the least problems. I suspect that these models are not very accurate. Only the real circuit will reveal the truth.When A2 did not have a negative voltage supply, Q3 had to have its base at a positive voltage. Now you can apply -1V to the base of Q3, even less to (V-)U2, then the current limiter will be able to operate for 0V at the output.LT1086 output current limit depends on voltageTest this circuit for different currents and voltages as well as load capacitance. Both in CC mode and CV mode. Change in current alters the transconductance of the transistors, which in turn changes the gain and bandwidth of the feedback loop, and thus the phase margin.

author: MisterHeadache
author_rank: Regular Contributor
timestamp: July 19, 2025, 04:28:49 pm
content: Quote from: MariuszD on July 19, 2025, 09:24:30 amThanks for running some additional tests for me! I also am playing around with various input voltages and loads and checking CC and CV stability, both in this AC sim and in my transient sim. So far, no new surprises. I did increase C1 (the feedback cap across Q1) from 1n to 10n, that helped further reduce some small oscillations I was seeing in my transient simulation, at the expense of some loop gain.Attached are my latest updated schematics - FEEDBACK PLEASE! One is for the rectifier board and the other is the main board. I have a third board, the 10mA load for keeping the LM317 in regulation, not included yet. I'm still tweaking values but am looking for any other future-proofing components that I should include.R15 (3 ohms) determines when the bypass transistors kick in. 3 ohms limits the LM317 current to around 1/4 amp. I'm trying to push the lion's share of the heat dissipation to the bypass transistors.