0-400V digital PSU design

[ronv]

Floating Ground

I'm not sure how to float the ground in Spice. Maybe Eric or someone with more knowledge of it can help.

You can download most devices for LT Spice. The trick is to find the model you want and then learning how to do it. I downloaded the high voltage transistors because I was worried about their leakage current. They will need a small heatsink.

Q1 is current limit. It turns off the pass transistor if the current gets to high.

It is still not clear to me what you are trying to accomplish so I'm not sure I am on the correct path.

All of these are self contained. I'm not sure that works for you.

 

[lordsandman]

my purpose is focusing an electron beam with electrostatic fields, like in the CRT tubes. metal plates act as lens system and change trajectory path. sequentially metal plate voltages referenced in sequence (grounded with another as i mentioned in post #11)

there is a bigger problem which i recently realised. when decrease the ref voltage to 0.15V (it corresponds ~6V output) Vout ripple changes shape. and there is a bit nonlinearity in Vdac-Vout relationship. how can this ripple and nonlinearity minimized?

 

[ronv]

Good catch.

We can make it better. Remove the 1k in the base of Q3, change R8 to 1k and add another 33Ufd. in parallel with the one on Vin. It can't go to 0 volts, but close.
I'm gradually getting what you are doing. The respose it not to fast. Is that a problem?

 

[lordsandman]

it works!! output has a ripple lower than 1mV and its quite linear. in fact, i fitted the dac-out graph to a linear function and its exactly linear by adj. R squared=1
i hope the circuit works like this in breadboard, cause i'm going to do this in a few days. with a difference, i'll use an ordinary 420V DC supply for unregulated voltage. i'll share the result in here

ronv, thank you very much for your patient guidance. do you recommend about selecting components or anything else?

 

[ronv]

I'm a little worried about the floating part. You will have a separate unregulated supply for each regulator? And a separate 15 volt supply for the op amp? What is the interface with the DAC? will each regulator have it's own DAC and micro or ????.

 

[lordsandman]

i suppose that there is a big time difference. my responses are late too sorry about that
yes, i will use seperate unregulated supply for each regulator. this is only for try out, at the final i will use rectifier. 12-bit R-2R DAC with current-voltage converter at the output will be the programming voltage. and 10.24V precise voltage referance for the DAC, so 1 LSB change at the DAC input corresponds 0.1V change at the output. every regulator will have it's own DAC. i'm planning a PIC that controls all of the DACs with an optocoupler for isolation. at the software side, i will use matlab for commanding PIC via RS-232. a have a figure of merit acquired from the system. so, i can optimize it by changing regulator outputs.
it may be neccesary that a complementary bipolar regulator outputs. can i use a resistor divider for obtaining complementary outputs from an unipolar one? for example, two ±200V outputs from a 400V unipolar?
what kind of transistors, resistors and capacitors should i use? are 2W %1 thin film resistors and 450V grade ceramic capacitors work? and worried about the pass element, which power transistor best suits the design?
is there a mininmum current requirement and what happens when short the output?
lots of questions

 

[ronv]

i suppose that there is a big time difference. my responses are late too

It's probably just as well. I keep finding improvements. The latest is to change R9 to 100 Ω. This increases the current limint to about 4 ma.

yes, i will use seperate unregulated supply for each regulator. this is only for try out, at the final i will use rectifier. 12-bit R-2R DAC with current-voltage converter at the output will be the programming voltage. and 10.24V precise voltage referance for the DAC, so 1 LSB change at the DAC input corresponds 0.1V change at the output. every regulator will have it's own DAC. i'm planning a PIC that controls all of the DACs with an optocoupler for isolation. at the software side, i will use matlab for commanding PIC via RS-232. a have a figure of merit acquired from the system. so, i can optimize it by changing regulator outputs.

Okay, sounds like we are good.

it may be neccesary that a complementary bipolar regulator outputs. can i use a resistor divider for obtaining complementary outputs from an unipolar one? for example, two ±200V outputs from a 400V unipolar?

Let me think about this.

what kind of transistors, resistors and capacitors should i use? are 2W %1 thin film resistors and 450V grade ceramic capacitors work? and worried about the pass element, which power transistor best suits the design?

There is nothing special. let me check wattage. I think we can make the 75K larger to reduce the power needed. and the 560K should be 1/2 watt. What will be the voltage range on your DAC? We may need to resize the feedback resistors to match. I just used 0 to 5 volts. You say the input will be 420 volts. What is the maximum required output?
I think the MJE18002 transistors will work but let me look at some others. Same with the op amp.

is there a mininmum current requirement and what happens when short the output?

There is no minimum because the voltage divider on the output supplies some load. When the current goes above 4 ma or so Q1 turns on and turns off the pass transistor. During a short there will still be a short pulse of high current, but I think the pass transistor may survive

 

[lordsandman]

What will be the voltage range on your DAC? We may need to resize the feedback resistors to match. I just used 0 to 5 volts. You say the input will be 420 volts. What is the maximum required output?

DAC voltage reference is 10.24V and maximum output is 409.6V, it's for easiness of software control. i will use 12 bit DAC(4096 steps) and in this values 1 LSB step at the DAC corresponds 0.1V at the regulator output

 

[ronv]

Hmm. Could be a problem. The circuit as it is won't quite give 409 v out with 420 in without the ripple going way up. We are pushing the transistor if we go much higher than 420 volts from the unregulated supply. I think we have 2 choices: Increae the input voltage from the unregulated supply and using a higher voltage transistor - I found a nice one but can't find a model yet. Or, If you can lower the maximum output voltage spec a little - say 390 volts, what we have will work. I have a little concern over what you will use for the unregulated supply. Do you have one in mind?
We have to keep in mind the simulation is not worst case, only typical so we need to leave some wiggle room.
I'll post the current limit simulations later today. Let me know about the supply voltages.
Where are you located?
I added the simulations for the current limit and the current for a short.
The current limit wanders around a bit with temperature due to the Vbe drop of the transistor but it should be ok. I added a resistor in the base of Q1 to limit the current just to be safe.
Do we need to build an unregulated supply?

 

[lordsandman]

i will use Kingshill 450V regulated supplies. they are old and have ~500mVrms ripples, but qualified supplies. there is no need to build unregulated, i can use them for every different grounded regulator outputs. 390V output a bit under of my desire. indeed, i think i can use 500V for Vin and ~500V max output if necessary, isn't it possible?

and in the circuit of mine 4mA output is stable
View attachment 62779

greetings from turkey

 

[ronv]

Okay! Found a nice high votage transistor FJP5027.
I made a few other "tweeks". Added R6 to limit short circuit current at high voltage. Added C1 R12 for stability. Change C2 for stability. Change R3 to lower op amp current.
Found a better op amp than the LM6142 - TLV2370. Has better temperature performance.
Lets play with it and see how it looks.

Turkey = cool. That is a few time zones.

This sounds like a lab project. Is it?

 

[lordsandman]

Okay! Found a nice high votage transistor FJP5027.
I made a few other "tweeks". Added R6 to limit short circuit current at high voltage. Added C1 R12 for stability. Change C2 for stability. Change R3 to lower op amp current.
Found a better op amp than the LM6142 - TLV2370. Has better temperature performance.
Lets play with it and see how it looks.

Turkey = cool. That is a few time zones.

This sounds like a lab project. Is it?

Hey ronv,
sorry about my very late response. i was outside the city and away from study. yes it is a lab project, but as hobbyist only. still i need stability and accuracy.
i have simulate your new design and get in trouble with 3rd party models. i added FJP5027, LM6142A and TLV2370 models from manufacturer websites and run with them. if i done this correctly the Vin and output is very strange for me. cause, i change the input (V1) voltage to 220V amplitude and 50Hz freq. also, there is nonlinearity between Vdac-Vout and large ripples which in the case Vdac<0.2V. when i used 2N5550 npn and LT1677 opamp output is very good. but i have no idea which in the case of long term stability and short circuit. could you send the models you have been used and proceed over the design which i'm not trouble within. here is the design which i used:
View attachment 63003

thanks again and again

 

[ronv]

Models

Now we are going to have fun, because I'm not very good at this.
The transistor is pretty easy:
Just copy this and paste it into LTC, LTc SpiceIV, LIB, CMP, LTSpice Bipolar. Now you can select it just like any other NPN in the exixting spice library.


.MODEL FJP5027 npn
+ IS = 1.84896E-10 BF = 26.0 NF = 1
+ BR = 1.8025 NR = 1.0 ISE = 1.04807E-9
+ NE = 2.0 ISC = 4.01764E-7 NC = 1.5
+ VAF = 58.7 VAR = 100 IKF = 0.9082
+ IKR = 0.39087 RB = 140.1 RBM = 0.0011
+ IRB = 1.01189E-6 RE = 0.00012 RC = 0.06183
+ CJE = 1.132025E-10 VJE = 0.711 MJE = 0.304
+ FC = 0.5 CJC = 1.08229E-9 VJC = 0.84
+ MJC = 0.25 TF = 9.6703E-9 TR = 3.342E-8
+ XTB = 1.12 EG = 0.60 XTI = 3

There are 2 zip file for the TLV2370. One is the subcircuit file the other the symbol file.
Follow the path above except at CMP go to SUB.. Create a new folder called NEW. Save the file TLV2370.sub into this folder as a text file.

Again follow the same path except instead of CMP or SUB select the SYM file. Again create a new folder named NEW. Save the TLV2370asc file here.
Now when you go to the component selection window in Spice you will see a catagory called New. you can click on the TLV2370 and insert it into the schematic.
I'll install spice on my other computer tomorrow and try it to make sure it works okay

 

[ronv]

My bad. Sometimes I get going to fast in testing.

The regulator needs some extra volyage in order to regulate. So increase your voltage closer to 500 volts. (Vin)

R11 needs to be changed back to 15 ohms.
R4 to 681K and R5 and 6 to 15.4K.
This will lower the power in the 681K and give a scale of about .45 volts per DAC step.
The resistor from base to emitter on Q1 is not needed.
Put R8 back in the base of Q2 to limit short circuit current.
Move the bottom of R5 and C5 to the output to get better regulation.
When you actually build it you won't need such large capacitors to filter after R11 since your supply only has a few mv of ripple.
I think we are good now but give it another check.
PS don't forget to add the .sub after the name when you save the sub file. That's what I always do.

 

[ronv]

One last thing - maybe 2.

If the 500 volt supply is on before the 15 volt supply the output will go to about 490 volts. Don't know if that is a problem in your application, but something to keep in mind,

Please be careful when you float one on top of the other as everything will be "hot".

 

[ronv]

Okay, I think we are bullit proof now.
Here are the tests I ran:
Ripple: Changed divider resistor to get 465 volts - .45 volts per DAC step. - R2 75K 5 watt C1, .47ufd. 5 volts of ripple in 2-3 mv out.
Current limit 3.2 ma minimum over temperature. Transistor inside SOA.
Fast rise time of 500v supply - stable. Transistor inside safe operating curve.
Slow rise or 500 volt supply - ok
Dac vs Vout - linear - stable in steps.
Vout vs current. Added feedback to compensate for drop across current limit resistor - R9
Short circuit - Transistors inside SOA. Added diodes for input protection of op amp (Most have therir own but we will see what's in your circuit)
The 75 K needs to be 5 watt, the 681K's 1.2 watt.
I can't think of any other things right now. Maybe you can.

 

[lordsandman]

it seems perfect i am out out the city now. when i arrive my land i will try it immediately. i am planning set the each DAC output as 2.5mV step. cause i will use a 12-bit DAC then, 10.24V/4096=2.5mV. i can produce it accurately

 

[lordsandman]

i tested it! it is absolutely wonderful. i can not find FJP5027 in locally. but i find KSC5027 (its fairchild too). main electrical characteristics are the same according to datasheets. but there are slight differences in the spice model. when i use KSC5027 model in LTspice the out seems to me much better. and i cannot find TLV2370 or LT1677. when i simulate with OP07 (as similar, low offset) output is very bad. which opamp can i use finally, TLV2370 or LT1677?

only a few details that i can bother. there is a little(%2 at min to max) nonlinearity, but i can adjust it within the software.
and when i use the rectifier as input, ripple increases at smaller output voltages. it may be important because i will use this supply for focusing electrons as i said. when the electron energy is as small as 3eV (it requires 3V supply output), it passes through other supply elements more slowly. so, it will affected much longer. i'd rather low ripple at 3V rather then 300V. but there is no problem in the case of DC input, so it will be ok!
i continue to playing with it. i'm trying to add DAC and digital models to spice. i'm providing the components. which type of capacitors should be used? i dont want use to electrolytic, may be polypropylene or teflon, i think.

KSC5027 model which i used:
View attachment 63142

 

[ronv]

Stability

Got me again. But I did learn how to do bode plots in spice.

We need to change R12 to 22K then it will be stable at low dac settings.

I think some of the non linearity you see is due to where you measure. You need to measure from -Vout to Vout or there will be an error due to current change across the current sense resistor. You can do this by clicking on "View, Set probe reference and placing the black probe on - Vout and the red probe on Vout. There is still some error but more like +/- .5%.

The op amp needs to be the rail to rail type as its output must get close to ground. So the things to look for are 16 volt supply voltage, Rail to rail with low bias current and drift.
One bode plot is for the dac to show it is now stable, the other for ripple.
I think for the Big caps electrolytic are fine. For the small ones I think ceramic would work ok. Use COG type with goof tolerance for the ones on the op amp. The output cap is not so important. The 681Ks and 15Ks will create an error that you may need to calibrate out, the others are not so important.

 

[lordsandman]

ok, thats my measuring mistake! the output characteristics are very well. i think it's time to consider about safety
there will be optocoupler between MCU and DAC. but still, a floating circuit like this can have safety issues associated with it due to the fact that there is no low impedance path to ground. also, when the PSU closed/no load, there is no way to discharge the capacitors. and there may exists capacitive coupling in transformer. or electrostatic discharge due to the other parts of circuit.
how they can be prevented? and would you detail your warning about directly connecting the outputs? the PSU which have floating output like this one should act as a battery