Isolated 12V supply

Discussion in 'General Electronics Chat' started by tom66, Sep 14, 2011.

  1. tom66

    Thread Starter Senior Member

    May 9, 2009
    2,613
    213
    I'm attempting to create an isolated 12V supply. This works from an 11V - 14.4V input (i.e. normal lead acid battery) and should produce about 12V @ 500mA. One essential point of this supply is that it *must* be isolated from the input because the other side is connected to the mains in some way.

    I've been working on this design in LTSpice, but it's hideously unstable. It starts off at 12V, but then sags down to around 4V, with very high ripple.

    Does anyone know why this might be so?
     
  2. tom66

    Thread Starter Senior Member

    May 9, 2009
    2,613
    213
    Ah! I noticed that my MOSFET was *always* on!!! I changed a few more things around and it seems more stable now.
     
  3. #12

    Expert

    Nov 30, 2010
    16,257
    6,757
    I did one very much like this using National Semiconductors Simple Switcher website calculator. Painless.
     
  4. tom66

    Thread Starter Senior Member

    May 9, 2009
    2,613
    213
    Are those fully isolated?
     
  5. #12

    Expert

    Nov 30, 2010
    16,257
    6,757
    Oops. My bad.
     
  6. iONic

    AAC Fanatic!

    Nov 16, 2007
    1,420
    68
    I would add one note with respect to the 12V Lead Acid Battery. It will never be at 14.4V unless you have just completed a bulk charge phase. After that point it will drop like a rock to 13.5V - 13.7V where ever your charger topping charge is set at. Once off the charger it will again drop over the next day or two, depending on the condition of the battery, to near 12.7V. Also, and more importantly, unless you do not care how long your battery survives, do not discharge it down to 11V as this will shorten its life a great deal. I wouldn't go below 12V before charging it. This may or may not affect the design you are working on.

    ...Of course all bets are off if this device is an emergency power off device and you REALLY need the energy. But an indicator of battery condition might be helpful in the circuit to signal that you have reached 12V and should charge the battery.
     
    Last edited: Sep 16, 2011
  7. t06afre

    AAC Fanatic!

    May 11, 2009
    5,939
    1,222
    Simulating this is one thing. But building it may be much harder. The problem will be the transformer. Unless you are sure you can get hold on a transformer with the correct spec.
     
  8. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    Hey Tom, you might find the attached interesting; an isolated DC-DC converter made using a 555 timer, optoisolator, and a toroidal transformer.

    It seems like it handles a widely variable load pretty well; 20mA or 500mA, it stays pretty close to 12v output.

    C5 needs to be 1/10th the value of C3 to ensure a soft start. You might try reducing it a bit if you'd like for it to start faster, but watch out for overshoot.
     
  9. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    Tom,
    I downloaded your simulation a couple days ago but didn't get to try it until yesterday evening. Did you really get it stable? I tried a few things, and it just wasn't looking too good.

    The OR/NOR gate needed to be replaced with an AND/NAND gate - I suppose you did that, along with some other things. Mind posting the circuit that you wound up with?
     
  10. tom66

    Thread Starter Senior Member

    May 9, 2009
    2,613
    213
    Oh, good point on the OR gate, I don't know why I made that an OR.

    I did eventually get it stable, even with the OR gate, which now I think about it, should never have worked... :eek: I've attached the *.asc. It's reasonably stable, but the output ripple is through the roof. I will be using a 78xx series regulator on the output though so don't see this being a problem. It will be powering some general purpose op-amps. I'll probably also add a negative rail, and a smaller tap for a 3.3V LDO, to run a microcontroller, but I'm getting ahead of myself.

    This version gives ~14.8V for 11 - 14.4V in, which is fine, anywhere from 12V - 18V out should be fine.

    I like the circuit you posted. I might use it, as I was going to use an op-amp for the oscillator anyway... why not use a 555 timer, as it is designed for it? :)
     
  11. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    Yes, I'm seeing terrible ripple as well as very high peak currents in the inductors. I'm not sure why that is at this point; some strange things are going on in that simulation.

    I'm not crazy about using the LTSpice built-in logic functions; you may not have noticed that they output either 0v or 1v, and for that reason I stopped using them once I found the 7400 and cd4000 libraries on the Yahoo! LTSpice group. It's likely you can make them output something else, but I haven't fiddled with them for years now - just never had a reason to look back. They're proprietary to LTSpice, so I'm hesitant to develop anything with the LTSpice-specific logic funtions.

    About that 555 version - I came up with that basic idea a year or so ago. The output voltage is really fairly stable for how simple the circuit is, although it'll be dependent on the temp of the optocoupler's emitter and it's Vf. Not bad though.
     
  12. tom66

    Thread Starter Senior Member

    May 9, 2009
    2,613
    213
    Here's my improved version.

    I've added additional rails, and figured out the driving logic. Much more stable, but still has very high ripple.

    I tried adding an LC filter, and it just goes crazy...

    Whilst an LDO may be able to filter it out, it is still a bit worrying.

    It's reasonably efficient. Total load is 3.79W + 3.34W + 3.11W = 10.24W and it's pulling about 14.9W, which is about 69% efficient. Could be better.
     
  13. iONic

    AAC Fanatic!

    Nov 16, 2007
    1,420
    68
    Hey Tom,
    Just extending my apologies for the battery lecture I gave you earlier on in the post. I must not have read the user-name before going on that rant. I'm sure you know exactly what your doing with respect to batteries.

    i
     
  14. tom66

    Thread Starter Senior Member

    May 9, 2009
    2,613
    213
    I haven't a clue about lead acid batteries! LiPo is my speciality, as I used them in my model aircraft, but even then I'm pretty clueless. You're quite right on the voltage range, 11V would be a pretty dead battery. This could be used in a car though; it's possible during cranking the voltage could drop as low as 6V, and this design can handle a brief under-voltage (for about 200ms, with a slight sag in output voltage but still sufficient.) No idea if this is good enough though as on a cold day it might take several seconds to start an engine.
     
  15. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    Tom,
    Did some more fiddling with your auxsupply simulation; see the attached.

    I had to adjust many resistor values; you were trying to sink way too much current with the LM339, you had forgotten that the LTSpice logic only goes to 1v, I replaced all of the "common" symbols with "G" just because I'm not used to using the common symbol, I added a snubber to the MOSFET drain, labeled a few points, made the schematic more compact so it was easier to view using the vertical format, and other misc. changes.

    I'm puzzled as to why the peak currents are so high in L1; they shouldn't be anywhere near that high, and there is no ramping up of the current like should be exhibited.

    You must be running on a Mac or on Unix, as every time I load an LTSpice simulation you've created, I get an "Â" (Latin capital A w/circumflex) before every "u", which I have to edit out. I don't know why that happens either, but unless I edit all of them out, I get really strange results from running a simulation.
     
  16. tom66

    Thread Starter Senior Member

    May 9, 2009
    2,613
    213
    I'm using VirtualBox Windows XP on Ubuntu. Maybe I should try uploading the file directly instead of copying it from Windows.

    The resistor between COM and GND should be 10Meg/1kV(+), for safety reasons, as it bridges the live (isolated) and battery side. On many power supplies I see two 4.7Mohm or 5.6Mohm in series.

    I've made a few changes to my version. Added your snubber idea and changed the resistors to limit sink current. Replaced the logic NAND and inverters with a transistor logic circuit (very very basic TTL, if you could even call it that :p), which definitely works better as the gate gets about 10V drive from an 11V input.

    I noticed that MOSFET was still experiencing very high peak voltages (~400V) even with the snubber; that wouldn't be particularly healthy for it! So I added a capacitor to shunt the hf to battery ground, which has mostly taken care of that (the peak voltage is 70V.) The cap should be poly or multilayer ceramic as it has to handle very high peak currents (up to 240A) and have a high working voltage; electrolytics will just nuke themselves.

    I don't know if LTSpice simulates MOSFET Vds breakdown, but as a precaution I selected an 80V MOSFET, which has quite good on-resistance of only 22mΩ, and low gate charge ~34nC, which is fine for this low power application. Maybe I should use a 100V MOSFET for some added margin, but this works well for now.

    After doing all of these changes, the peak current in the primary winding is now just 30A, with a limited spike before the ramp. It looks much more like a switching regulator should do. Also, the efficiency is now around 80%, instead of 60%, which is good for me. The MOSFET dissipates about 1.2W, and is probably the highest loss in the power supply. A good heatsink will be needed, and I will look out for a good TO-220 device. In the potential application (which shall remain a secret for now :p) there are two large heatsinks, one primary and one secondary, which other power components will be bolted to; a fan will then blow air through these heatsinks to keep the devices cool. There will be several power MOSFETs (70A+ per device) on the heatsink, which will be dissipating around 60W at peak power, so effective cooling shouldn't be an issue. Well, if it is, then I could say goodbye to those power FETs!!

    I've gotta think how a transformer might be wound to use this. I'm thinking of ripping a transformer out of a dead PC power supply and re-winding it. This is just an idea for a little project, and it may never reach fruition, but it would be interesting to see if it actually works.

    I'll upload the actual asc from Windows, stand by...
     
  17. tom66

    Thread Starter Senior Member

    May 9, 2009
    2,613
    213
    I come bearing an *.asc.
     
  18. tom66

    Thread Starter Senior Member

    May 9, 2009
    2,613
    213
    Okay, so in my spare time I've been working on the power supply design.

    The next task is to get it handling 60V transients, as common on automotive systems.

    The output ramps itself up to ~90V when the transient hits. Ideally, it would remain in regulation, at worst it would stop outputting... but this thing would fry any secondary side semiconductor.

    It seems as if the oscillator/gate goes a bit out of control whenever the transient hits.

    Any ideas?

    (I'll attach the *.asc in a min.)
     
  19. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    Tom,
    I spent some more time yesterday evening fiddling with your latest simulation incarnation. (intarnation? ;) )

    You should move the B+ net label from above V1 to somewhere in the vicinity of C1.

    I'm still getting very high current through the MOSFET and inductor, and I'm not sure why yet.

    C20 increases the peak current through M1 considerably, as it doesn't have a diode and bleeder resistor like the snubber combo D3/R17/C19.

    The TVS diode doesn't seem to be clamping very effectively.

    You had V2 (gate square wave source) set to 5kHz @ 50% duty cycle. That seems quite low for a 250uH primary winding. Having the frequency so low means you'll need a large transformer core, and lots of windings; it will likely be audible as well. You should really get the base frequency to >30kHz to enable reduction of the trafo size and core losses.

    Your design keeps getting more and more complex, but for some unknown reason you seem to have forgotten about the duty cycle percent of V2. Right now, it's effectively 50% or 0%. That makes control of the output voltage very coarse.
     
Loading...