Check my PSU design and LTspice sim - diyAudio
Go Back   Home > Forums > Amplifiers > Power Supplies

Please consider donating to help us continue to serve you.

Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving
Reply
 
Thread Tools Search this Thread
Old 22nd June 2007, 09:09 PM   #1
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
Default Check my PSU design and LTspice sim

I have designed a four-output regulated DC power supply, with +/-30VDC 5A-max and +/-18VDC outputs.

I'd like some feedback about it, especially if anyone sees anything wrong with it, or has any suggestions for improving it.

I haven't built it, yet, but will probably build one to try it as the power supply for a chipamp-based audio power amplifier.

For everyone's convenience, I have posted both the schematic and the downloadable LTspice files for the power supply on my "LTspice stuff" webpage, at:

http://www.fullnet.com/~tomg/gooteesp.htm

Thanks.

Regards,

Tom Gootee

http://www.fullnet.com/~tomg/index.html
  Reply With Quote
Old 23rd June 2007, 11:45 AM   #2
AndrewT is offline AndrewT  Scotland
diyAudio Member
 
Join Date: Jul 2004
Location: Scottish Borders
Hi Tom,
I am surprised at the improvement in output ripple from adding the third 4.7mF smoothing cap.
This leads me to suspect that there is something else going on that is not being properly simulated.
Your circuit is all very conventional except for the secondary current limiter. Is the FET safe with 15Vgs and max voltage across DS? Does 33k & 22u allow full current after about 1second? How does the Zener affect this time constant?
Why use a Pfet in the upper most rail? Would an Nfet work if it were moved to the lower positive supply rail (just like the negative supply)?
Did you reject using a Power Thermistor as your current limiter?
Are your specs for the various electrolytics fairly "normal" or are these "super spec" (equivalent to low ESR or some such)?

Further research: add uohms (or even mohms) to the ground leads between each of the connections. Then see if ripple etc deteriorates.
Disconnect the main smoothing ground before each of the regs and reconnect it to the output ground for the respective regs, again with appropriate uohms in the ground connections. Does that alter/improve the output quality?
When you disconnect/move the smoothing ground from the regulator ground you will need to add the minimum input capacitance that each manufacturer recommends for every regulator.

Q.)
what are the units in the leakage current formula Ileakage<=0.01CV if C =Farads & V =volts I always find that leakage is predicted as about one hundred to 1000 times worse than what I measure when I have done a test through a high resistance feed. Or does the leakage only approach the worst case when applied voltage is at or near the maximum working voltage? or is that something else I don't understand?
__________________
regards Andrew T.
  Reply With Quote
Old 23rd June 2007, 10:34 PM   #3
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
Thanks, Andrew! Those are the types of comments and questions I was hoping to get.

I had started with an IRF4905 P-channel MOSFET for the soft start in the positive rail, which is good for Vgs <= +/-20v, but changed to the STP80PF55 because it was much cheaper (when it showed up as an "equivalent" during a search for the IRF4905 at mouser.com). It can handle Vgs <= +/-16v. So maybe that's cutting it too close and a slightly lower-voltage zener than 15v should be used? THE MOSFETs should be fully on when Vgs's magnitude is more than 4 volts or so, I think. The STP80PF55 can handle 55V and 80 amps, and has an Rds(on) of 0.016 Ohms. So it should be fine, otherwise. The corresponding N-channel MOSFET for the negative rail is similarly rated, except it can handle Vgs <= +/-20v and has an Rds(on) of 0.005 Ohms.

With the 33k/22uF, both MOSFETs get to full current in about 0.7 seconds, effectively removing the parallel 1-Ohm resistors from the circuit, after startup. The Zeners don't affect the time constants at all, as far as I can tell (having tried the simulation without them). The MOSFETs should be fully "on" well-before the zener voltage is reached. The zeners were put there only to limit Vgs to keep it within each MOSFET's "absolute max" spec, since the rails will exceed those.

I don't know how to use an N-channel MOSFET for the positive rail. That "lower positive supply rail" is 0v.

And yes, I guess I did sort-of reject using an NTC thermistor as the current limiter. (I have used them before.) Maybe I'm being too lazy, or am being unreasonable in feeling they are too "messy" design-wise, but, short of testing a lot of them (and I do have many free samples of them, here), I can never seem to find enough data for them, to enable me to easily predict the variation in resistance vs current. And I just get the feeling that the resistance might vary "too much", over, say 1A to 5A, if using a thermistor. With an FET, I _know_ what the resistance will be. And if I DO want some more resistance in there, I can just add a known-value resistor.

(Note that I _have_ worked with the smaller types of NTC thermistors, quite a bit, for temperature-compensation design purposes. And I did work out an "easy" way to linearize them, or otherwise tailor their responses, using LT-Spice, at least for the Epcos thermistors, for which they provided a very nice spice models library that uses the standard thermistor equations and even includes self-heating effects. So "maybe" I could try to apply some of that experience to the larger inrush-limiter types, and could try to design a thermistor-resistor network that gave a desired resistance curve versus current, etc etc. But that sounds like a lot of work (even just for finding out if it's necessary to even worry about it), compared to just using the FET circuits.) But, maybe, some day, when I'm not feeling as lazy, I will go measure, or even just try in this circuit, some of the NTC inrush-limiters, since they do seem to be commonly used, and it might be a better solution. The cost would be lower and they would use less PCB real-estate.

The Nichicon UHE-series electrolytics, which are what I often use, now, whenever electrolytics are needed, are somewhat-special "low-impedance high-reliability" types, but are very-reasonably priced, IMO, at mouser.com. The 22uF/50V are $0.15 qty 1, for example. And a 2200uF/50v UHE-series would be only $1.81 qty 1. The UHE series' larger-sized and higher-voltage models are rated at 10000 hours life, _when_ operating at 105 degC with their max rated ripple current and at their max rated voltage. Even their lowest-voltage and smallest-sized models are still rated at 4000 hours, under similar conditions. (Aside: I also particularly like the Nichicon UHE-series 3300uF/35V caps, rated at ESR .013 Ohms at 100 kHz, and 4.08A RMS ripple at 100 kHz, with 16mm D x 40mm H, LS 7.5 mm, for $1.69 qty 1.)

The United Chemi-Con KMH-series just happen to be what I typically use for power supply input smoothing caps. The 4700uF/63V models are spec'd as having 0.053 Ohms ESR at 120 Hz at 20 degC. There are two sizes available, for that value, currently priced (at mouser.com) at $3.12 qty 1 for 25mm diam x 50mm H, and $4.32 qty 1 for 30mm diam x 40mm H. (Aside: I also like the KMH-series' 12000uF/35V model with .035 ESR(120Hz) for $3.41 qty 1, and the 33000uF/35V with .012 ESR(120Hz) for $9.16 qty 1.)

I, too, was wondering about the ripple-voltage's improvement, when changing from 2X 4700 uF to 3X 4700uF. It didn't seem all that unreasonable, to me, at the time. But that type of thing is one reason why I asked for comments and opinions. I did previously simulate the same basic supply circuit, but with only 1uF or so on the regulators' adjust pins and no soft-start circuitry, for the three cases with 1X, 2X, and 3X 4700 uF smoothing caps, and saw fairly-analagous ripple-voltage improvements. If the ripple improvements' magnitudes are NOT entirely reasonable, then I should be looking for something that's not modeled well-enough. (Also see my comments about trace/wire parasitics, farther below.) But I was hoping that the 47uF (with 2.26 Ohms ESR @ 120Hz) on the ADJ pins might be responsible for the good ripple specs. I guess I will also see what happens when I build one, and try it with both 2X and 3X 4700uF smoothing caps.

NOTE that in the LT-Spice schematic given, you can right-click on each component, to see what parasitics are included for the simulation. For example, each electrolytic capacitor includes the ESR (equivalent series resistance) at 120 Hz, plus a guessed-at-for-now ESL of 9 nH, and an equivalent parallel resistance (1/.01C) to try to model leakage current. I usually also include a parallel pure capacitance for each resistor (typically 0.3pF or 0.5pF), but did not do so for this schematic. And when inductors are present, I always include at least their DC resistance. (Note that for AC Analysis, it is also possible to include a capacitor ESR model that varies with frequency, using Laplace sources.)

Re your "further research" comments:

I will try the things you have suggested. I didn't put anything like that, in THIS model. But I typically DO add both resistance and inductance in almost ALL leads and traces, for my "real" simulations. And once I start designing a PCB, I calculate or measure the actual trace resistances and inductances, and include those in the model. They can make a big difference.

Even more "interesting" is testing such a supply with a dynamic load! For that, I have often used the OPA541E ("E" model-version) chipamp model (from ti.com), also available from that page (i.e. at http://www.fullnet.com/~tomg/gooteesp.htm ), configured as a simple power amplifier, pumping, for example, max-voltage square waves into a low resistance (e.g. drawing near the supply's current limit; Note that square waves are slew-rate limited to within chipamp's spec.).

When the parasitic trace and wire inductances and resistances are included, that type of (dynamic load) simulation can be VERY valuable (and can also help, a lot, in picking the "best" power supply bypass circuits for the amp, for example). And for the "star ground challenged" among us, it will definitely make believers out of them!

Aside: Note that I included a rudimentary example of a star ground simulation setup, for starting those types of investigations (i.e. with ground-returns' and supply leads' impedances), in the "DC Servo" schematic on that same web page. (Note also that, when using setups like that, you sometimes can run into Spice "algorithm convergence" problems, and often have to play around with the Spice "internal" solver settings in the LT-Spice Control Panel, or tweak your parasitic values, to get them to run, or run with reasonable speed, which can sometimes become rather maddening.)

The units for the leakage formula are Farads and Volts, I assume. The Nichicon UHE-series' datasheet says "After 2 minutes' application of rated voltage, leakage current is not more than 0.01CV or 3 (A), whichever is greater." I have never actually measured capacitor leakage current, or done much research on it. So I don't know how well that formula predicts it, or under what conditions it's valid, etc. I'm glad to hear that it usually measures as less than predicted, for you. But what's that about "through a high resistance feed"? Couldn't your "high resistance" be limiting the leakage current? Maybe you should try using a potentiometer, and then slowly lowering the pot to around zero ohms after the cap has charged, and then measuring the leakage current. Just a thought.

I HAVE had cases where the calculated leakage current was LESS than 3 uA, but have never accounted for that in any power supply simulations, assuming it was insignificant. (However, for a high-precision feedback loop's capacitor, for example, I might want to try to account for it.)

Thanks again, Andrew. I realize that this power supply's design is basically bog-standard, except maybe for the soft-start, which was more-or-less necessitated by the relatively-large caps on the main regulators' ADJ pins. I was also wondering if anyone thought that those caps were too large, and if there was something wrong with doing it that way.

Also, I just thought it might be a good idea, in general, to post complete "ready-to-run" LT-Spice circuits, so others could simulate them, for themselves (possibly making circuit discussions much more fruitful), and also just to try to make it easier for people who might then get started using LTspice, since it's usually easier to modify someone else's existing circuit than to try to start from scratch.

Regards,

Tom Gootee

http://www.fullnet.com/~tomg/index.html
  Reply With Quote
Old 23rd June 2007, 10:51 PM   #4
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
Quote:
Originally posted by AndrewT

<snipped>
Disconnect the main smoothing ground before each of the regs and reconnect it to the output ground for the respective regs, again with appropriate uohms in the ground connections.
<snipped>
I don't understand what you mean, here. The positive rail's ground already goes all the way from its' rectifier bridge to the load. And the negative rail's "smoothing ground" goes to its' regulator's input, and can't be connected to the output ground, since the negative rail's "smoothing ground" sits at about 2.8 volts.
  Reply With Quote
Old 24th June 2007, 12:07 AM   #5
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
Quote:
Originally posted by AndrewT
Hi Tom,
I am surprised at the improvement in output ripple from adding the third 4.7mF smoothing cap.
This leads me to suspect that there is something else going on that is not being properly simulated.
<snipped>

Further research: add uohms (or even mohms) to the ground leads between each of the connections. Then see if ripple etc deteriorates.
<snipped>

Hi Andrew,

As a quick test, I added "100nF in series with 0.001 Ohm" (roughly four inches of some size of wire or PCB trace. 20ga wire?), between each output and the load resistors, and between the junction of the load resistors and the Common, and also between the positive rail's regulator's "ground" and the Common, and between the negative regulator's output and Common. I also added "25nH in series with 0.00025 Ohm" (roughly one inch of some wire or PCB trace) on both sides of each end of each smoothing cap, and also after each side of both rectifier bridges.

I ran sims with that setup for the 3.5A, 4A, and 5A load currents, since those had shown a lot of difference in the ripple voltages between the 2X and 3X 4700uF cases. Ripple voltages were measured at t = 2 seconds.

For _3X_ 4700uF, the +/-30V rails' p-p ripple voltages with 3.5A loads went from 211uV/217uV (without added wiring parasitics) to 208uV/214uV (with added wiring parasitics); an improvement. For the 4A loads they went from 235uV/241uV to 229uV/238uV; an improvement. And for the 5A loads, they went from 103mV/654uV to 111mV/725uV.

For _2X_ 4700 uF, +/-30V rails' p-p ripple voltages with 3.5A loads went from 1.0mV/665uV to 1.1mV/687uV. For 4A loads: 150mV/73mV to 156mV/79mV. For 5A loads: 424mV/380mV to 427mV/383mV.

So, not much change. But maybe it was a badly designed experiment. (ALSO, I realized, after making these measurements, that after taking the original measurements as posted on the webpage, I had added a 0.22uF film cap in parallel with each of the 47uF caps on the two main regulators' adjust pins.)

- Tom Gootee

http://www.fullnet.com/~tomg/index.html

EDIT: It looks like the resistance I used should have been about 4X as much per inch. I will try that and will report back if there's much difference.
  Reply With Quote
Old 24th June 2007, 12:08 AM   #6
AndrewT is offline AndrewT  Scotland
diyAudio Member
 
Join Date: Jul 2004
Location: Scottish Borders
Quote:
Originally posted by gootee
I don't know how to use an N-channel MOSFET for the positive rail. That "lower positive supply rail" is 0v.................
"After 2 minutes' application of rated voltage, leakage current is not more than 0.01CV or 3 (A), whichever is greater." ........... But what's that about "through a high resistance feed"? I HAVE had cases where the calculated leakage current was LESS than 3 uA, but have never accounted for that in any power supply simulations, assuming it was insignificant. (However, for a high-precision feedback loop's capacitor, for example, I might want to try to account for it.).......................


http://www.fullnet.com/~tomg/index.html

Quote:
Originally posted by gootee
I don't understand what you mean, here. The positive rail's ground already goes all the way from its' rectifier bridge to the load. And the negative rail's "smoothing ground" goes to its' regulator's input, and can't be connected to the output ground, since the negative rail's "smoothing ground" sits at about 2.8 volts.
Testing a perfect capacitor for leakage would result in zero current. If a resistor were placed in series with the DC supply and the test capacitor then there would be zero volts drop across the resistor once the capacitor has charged up.
But we don't have perfect zero leakage capacitors.
Now increase the resistor value and increase the DC supply value so that the capacitor just reaches it maximum working voltage. Now measure the voltage across the resistor. Eg. 15mF 63Vdc cap with 100k series resistor fed from 63Vdc will never reach 63v across the cap. I had to raise the voltage to about 65V just to get to 60V across the cap leaving a measured Vr=5V. Ileakage=5/100,000=50uA. Predicted Ileakage =0.01*15*10^-3*60=9000uA. I had to use a regulated supply for this since it can easily take 24hours to reach steady state conditions. Using a variac and transformer to feed the test cap resulted in hour by hour variations in supply voltage which ruined any attempt at measuring the Vr.

With a dual winding/dual rectifier PSU the regulator can be inserted in to either the upper supply leg or the lower supply leg. Similarly the current limiter could be placed in either supply leg. This would allow an Nfet (cheaper and higher spec) to be used for both positive and negative supplies. After the regulators the grounds can then be connected.

Looking at the positive regulator, the smoothing ground is connected to the adjust pin resistor and then feeds this reference all the way through a dozen other connections before reaching the load return. The Load should be returned to near the adjust reference. But this still allows ripple in the smoothing caps to feed through past the adjust reference to the load. The connection from smoothing ground must be broken before it reaches the adjust reference and instead taken direct to the load return star connection. If you insert the micro resistances in the ground wires, this ripple through should be simulated and you should also be able to see the improvement from relocating the smoothing ground to the return star.
Looking at the negative supply. The "ground" only starts at the output pin. Prior to the regulator the input "floats" at a variable voltage that is totally dependant on the regulator drop. If you see just 2.8V drop across the regulator then you may be suffering output droop due to supply ripple allowing the regulator to "drop out". This may account for the apparent massive improvement in output ripple when the extra 4.7mF is added. It may be that the lower ripple prevents the regulating action dropping out.
__________________
regards Andrew T.
  Reply With Quote
Old 24th June 2007, 12:57 AM   #7
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
Quote:
Originally posted by AndrewT

Looking at the positive regulator, the smoothing ground is connected to the adjust pin resistor and then feeds this reference all the way through a dozen other connections before reaching the load return. The Load should be returned to near the adjust reference. But this still allows ripple in the smoothing caps to feed through past the adjust reference to the load. The connection from smoothing ground must be broken before it reaches the adjust reference and instead taken direct to the load return star connection. If you insert the micro resistances in the ground wires, this ripple through should be simulated and you should also be able to see the improvement from relocating the smoothing ground to the return star.
Ok. I understand. I usually do things that way (see the DC Servo example's grounds, at http://www.fullnet.com/~tomg/gooteesp.htm ). But this was still just a more "conceptual" schematic.

For the positive regulator, I've broken the connection between the smoothing caps' ground and the regulator's adj-pin cap's (and its divider's) ground, and have routed those grounds separately to the disconnect network, so they don't share a common path and so I can insert a different impedance into each of them, and have done the same thing for the load return, the +/-18V ground, and the negative regulator's output (ground).

Quote:
Looking at the negative supply. The "ground" only starts at the output pin. Prior to the regulator the input "floats" at a variable voltage that is totally dependant on the regulator drop. If you see just 2.8V drop across the regulator then you may be suffering output droop due to supply ripple allowing the regulator to "drop out". This may account for the apparent massive improvement in output ripple when the extra 4.7mF is added. It may be that the lower ripple prevents the regulating action dropping out.
I had thought of that, but didn't think 2.8V would do that, with an LT-1084. I can find out by simply lowering its output voltage and comparing some of the 2X and 3X 4700 uF cases, again.

I have to leave, for tonight (It's 7:15 pm on Saturday.). So I'll get back to this tomorrow.

Thanks again, Andrew.

- Tom Gootee

http://www.fullnet.com/~tomg/index.html
  Reply With Quote
Old 24th June 2007, 04:23 PM   #8
BWRX is offline BWRX  United States
diyAudio Moderator Emeritus
 
Join Date: Jan 2005
Location: Pennsylvania
As Andrew mentioned, it would be more economical to use the same inrush current limiter for each rail. I would use the P-channel version and change your zeners to 12V. Alternatively, you could just use the standard relay and parallel resistor inrush limiter on the primary of the transformer. Nothing wrong with the tried and true method.

Since you're using regulators with good 120Hz ripple rejection (the LTs are great here with the adj cap), why not move one of the 4700uF caps before the reg to after the reg? This will lower inrush current a little, reduce cost a little (now you don't need the 220uF caps), and will help stiffen the regulated output voltage without hurting the ripple figure that much.

Remember that the 3 terminal regs have a fixed voltage between the output and adjust pin, so a variable resistance for R2/R15, R6/R16 will give you a variable programming current for different output voltages. It's probably best to use fixed resistors there and put a potentiometer in parallel with R3, R7 to fine tune the output voltage.
__________________
Brian
  Reply With Quote
Old 25th June 2007, 10:25 PM   #9
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
Hi Brian,

Quote:
Originally posted by BWRX
As Andrew mentioned, it would be more economical to use the same inrush current limiter for each rail. I would use the P-channel version and change your zeners to 12V. Alternatively, you could just use the standard relay and parallel resistor inrush limiter on the primary of the transformer. Nothing wrong with the tried and true method.
I hate to keep displaying my ignorance, but, I still can't figure out how to swap one of the regulators to the opposite side of its secondary, when only positive regulators are available.

Quote:
Since you're using regulators with good 120Hz ripple rejection (the LTs are great here with the adj cap), why not move one of the 4700uF caps before the reg to after the reg? This will lower inrush current a little, reduce cost a little (now you don't need the 220uF caps), and will help stiffen the regulated output voltage without hurting the ripple figure that much.
That's probably not a bad idea. I haven't played with simulating dynamic loads enough, yet, to know how raising the 220uF on the regulators' outputs might improve the supply's performance.

Trying it, just now, with an OPA541E model connected to the PSU's rails (with bypassing caps of 220uF/1uF/0.33uF/0.01uF), pushing 18V p-p slew-rate-limited square waves through a "mixed" load (40R || 100R--1uF) (just what I happened to have in there, for something else I was doing), I see that the transients on the positive rail are reduced in amplitude by about 20%, when the reg's output C is raised from 220uF to 1000uF.

Quote:
Remember that the 3 terminal regs have a fixed voltage between the output and adjust pin, so a variable resistance for R2/R15, R6/R16 will give you a variable programming current for different output voltages. It's probably best to use fixed resistors there and put a potentiometer in parallel with R3, R7 to fine tune the output voltage.
Thanks. I knew about the adjustment, of course. But I usually just used a 200 Ohm trimmer potentiometer for the upper 100-Ohms-nominal resistance in the regulators' output dividers. Your idea of using a pot in parallel with fixed resistors is better, probably giving finer control for a pot with fewer turns available, while also improving the circuit's reliability.

- Tom Gootee

http://www.fullnet.com/~tomg/index.html
  Reply With Quote
Old 25th June 2007, 10:32 PM   #10
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
I have added a download link for an "improved" version of the Quad PSU's schematic to my "spice stuff" webpage, at:

http://www.fullnet.com/~tomg/gooteesp.htm

This newer version has separate ground return paths, for most of the grounds, with a star ground point, more like a real circuit might be constructed.

With this setup, we can investigate what happens if ground return currents share the same wire or trace, and can see the effects of using different wire or PCB-trace lengths and sizes.

I have provided a link for downloading the LT-SPice file for the schematic, as well as a link to just a JPEG picture of the schematic.

- Tom Gootee

http://www.fullnet.com/~tomg/index.html
  Reply With Quote

Reply


Hide this!Advertise here!
Thread Tools Search this Thread
Search this Thread:

Advanced Search

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are Off
Refbacks are Off


Similar Threads
Thread Thread Starter Forum Replies Last Post
PSU Design Check Please ANDYLASER Power Supplies 14 15th July 2010 12:42 PM
How many people here use simulators, like LTspice, to help design tube stuff? hotbottle Tubes / Valves 6 18th March 2008 06:33 PM
What software except ltspice for schematics design (no simulations, just layout) DonOE Everything Else 3 8th October 2006 07:23 PM
New Here. Will you check me design? SightSeeker1 Subwoofers 19 13th April 2006 04:59 PM


New To Site? Need Help?

All times are GMT. The time now is 07:54 PM.


vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2014 DragonByte Technologies Ltd.
Copyright 1999-2014 diyAudio

Content Relevant URLs by vBSEO 3.3.2