UC3843

[metal]

Hi,

I am trying to design a boost converter that outputs 270V from 12V using UC3843, the design is attached, but I am not sure if it 100% correct, feedback is appreciated. Also, what is the reverse voltage so I can decide on the  schottky diode to use for THT?

[vern]

reverse voltage would be 270V, a 300V schottky should be fine.

[Checksum8]

These are two diodes I use a lot. Both are ultra fast. For surface mount ES1F (300v 1A) or ES1G (400v 1A). Through hole UF4004 (400V 1A).

[optikon]

I put your circuit into Microcap for simulation.

The error amp is at 2.5V.

As such, I used your 170k as109k to achieve 275V output -- unloaded.

The simulation seems to work fine.

In my sim, I used output capacitor as only 5uF to speed up the simulation at no load.

Since you will be driving 25mA, you do need much more C and higher target voltage to get to 25mA @ 275V

[PM3295]

The inductor value is a bit high.

This is what I calculated:

********** Input Data **************
Vout:= 270 V

Iout:= 25 mA

Eff:= 0.8

Vin_min:=11 (assume min 1 V drop over device)

UC3843_max_D:= 0.96
************************************

Max_Ton:= 1/103E3 * 0.96
Max_Ton =[9.3204 us]

Win := (Vout * Iout)/Eff
Win =[8.4375 W]

Iav:= Win/Vin_min
Iav =[767.0455mA]

Ipk:= 2 * Iav
Ipk =[1.5341 A]

L:= (Vin_min * Max_Ton)/Ipk
L =[66.8306 uH]

*********** Test case L = 100 uH *********
L:= 100E-6
di:= 1.5341
dt:= 10E-6 - 9.32E-6

Vout:= L * (di/dt)
Vout =[225.6029 V]--> Too low

Since the UC3843 is operating at > 50% D, slope compensation will be needed for stability.

Optional: Use smaller L value to keep D below 50%. Keep in mind peak currents will be higher.

[optikon]

The sim with L = 47uH and some realistic parasitics, still shows serious regulation problem at 25mA (@275V) load

EDIT: fixed typos..

Found in sim that L = 33uH, R divider = 104.7k with 1k with Cout = 150uF achieves 275V @ 25mA
Also had to use a lower RDS(on) MOSFet and  lower the Isense resistor.

Not sure if the model can be trusted but it sort of is making sense.

[PM3295]

Here is the sim verification of my previous calculated values

Posted on: October 03, 2020, 03:54:58 03:54 - Automerged

Found in sim that L = 33uH, R divider = 104.7k with 1k with Cout = 150uF achieves 275V @ 25mA
Also had to use a lower RDS(on) MOSFet and raise lower the Isense resistor.

Not sure if the model can be trusted but it sort of is making sense.

If your duty cycle is near 50 % or more, you risk having instability (sub harmonic oscillations). So check the gate pulse shape to make sure
there are no bursts of wide pulses, indicating stability issues.
 

[PM3295]

 {**** Case for max duty cycle without slope comp*** }
Vout:= 270
Iout:= 25E-3
Eff:= 0.8
Vin_min:=10.5 { 1 V drop over (I)Rsense and 0.5 V over MOSFET }
max_D:= 0.49 { 49% - Many designers try and stay away a bit further for safety ~ 45% }

{*** Needs slope comp for D >= 50 % ***}

Max_Ton:= 1/103E3 * max_D
Toff:= 1/103E3*(1-max_D)
Toff =[4.9515u]
 
Max_Ton =[4.7573u]

W_needed:= (Vout * Iout)/Eff
W_needed =[8.4375] {Watt}

Iav:= (Watts_needed/Vin_min)/max_D
Iav =[1.6399]

Ipk:= 2 * Iav
Ipk =[3.2799]

L:= (Vin_min * Max_Ton)/Ipk
L =[15.2296u] { Max value of L without slope comp }

di:= Ipk
dt:= Toff - Max_Ton

Vout:= L * (di/dt)
Vout =[270.2624] {Volts}


Sub-harmonic oscillation will be clearly visible in a bode plot of the transfer function of this converter (62 % duty-cycle) as shown below.

[optikon]

PM3295 simulation is much more meaningful than the one I put together, I didnt put much thought into the design itself just that it could run in Microcap.

Its nice to see Simetrix can run it too.

PM3295, where did you get that design procedure you have worked through?

From the datasheet or a Book ref?

Thanks

[PM3295]

PM3295, where did you get that design procedure you have worked through?

From the datasheet or a Book ref?

Thanks

The calculations are based on standard transfer function equations, that you can find in almost any power electronics text book. You can also derive them from first principles, if you know the basic energy storage equation of an inductor (LI^2/2).
 

Posted on: October 03, 2020, 03:34:35 15:34 - Automerged

I put your circuit into Microcap for simulation.

The error amp is at 2.5V.

As such, I used your 170k as109k to achieve 275V output -- unloaded.

The simulation seems to work fine.

In my sim, I used output capacitor as only 5uF to speed up the simulation at no load.

Since you will be driving 25mA, you do need much more C and higher target voltage to get to 25mA @ 275V

There is no need for a large cap in this case. It pushes the control bandwidth very low and make stability control more of an issue.

Below is the ripple with only a 10 uF cap. I don't think 27 mVpp is any problem.
 

[metal]

Thank you!

can you please upload sim files, thanks a lot indeed, I never expected to see this discussion!
How did you get US3843 into the simulation Microcap? I am not very familiar with Microcap, barely watched a video yesterday to see how to it can be used. Can I see these results in Microcap as well?

Also, how can I measure delta IL, ripple, etc I am willing to achieve 1mV ripple if possible.
Thank you!

[PM3295]

Will your load current be constant, or vary? If not constant, what will be the variation?

[optikon]

Thank you!

can you please upload sim files, thanks a lot indeed, I never expected to see this discussion!
How did you get US3843 into the simulation Microcap? I am not very familiar with Microcap, barely watched a video yesterday to see how to it can be used. Can I see these results in Microcap as well?

Also, how can I measure delta IL, ripple, etc I am willing to achieve 1mV ripple if possible.
Thank you!

PM3295 is using Simetrix, not Microcap. but he is looking deeper into the design performance and stability.

I  put a working sim together in Microcap, with no effort on the design. The output cap in the microcap sim has an IC condition on it to settle near final value quickly.. you can remove that if you want to see the whole startup.

Also, I agree with using the smaller output cap based on the ripple you can tolerate.

Maybe PM3295 can upload his Simetrix project also to play with.

EDIT: Microcap 12 project attached - its a working sim, but your design needs some work/adjustments per PM3295 findings..

[PM3295]

Maybe PM3295 can upload his Simetrix project also to play with.

I can upload the design file once we know all the design requirements (ripple, load current variation.. etc.)

Here is a Proteus file, (which metal likes) to play with in the mean time.

[PM3295]

With a two-stage  output filter, you can achieve very low output ripple.

I initially made R2 smaller at 100m ohm to start up faster in the sim. In practice, R2 should be around the 220m to 270m range.

[metal]

Requirements:
Vout = 270V
Iout = 25mA
Ripple = 1mV

I am unable to get this simulation to run correctly in microcap, what am I doing wrong?

[PM3295]

Will Iout be constant at 25 mA? What type of load is this?

[metal]

tube

If simulation takes a long time in microcap, how can I make things faster? is it possible to start simulation after 1 second so things are stable?

[optikon]

Requirements:
Vout = 270V
Iout = 25mA
Ripple = 1mV

I am unable to get this simulation to run correctly in microcap, what am I doing wrong?

I uploaded a working microcap project. did you try it?


Posted on: October 03, 2020, 11:43:35 23:43 - Automerged

tube

If simulation takes a long time in microcap, how can I make things faster? is it possible to start simulation after 1 second so things are stable?

Sometimes the periodic operating point option can speed things up. But the controller model has elements inside of it that are incompatible. so your only option is to put an initial condition on your output cap so that most of its charging to steady state is already complete. this requires you predict it and iterate.

Another approach is to just let the cap be much smaller and dont worry about the ripple you will see as long as the DC is correct. when everything is tuned right and stable, you can then work on the ripple.. or just wait for your breadboard.

[PM3295]

I have not used MC in the last five or more years. This is not a good tool for SMPS analysis with a switching model. What a frustrating experience. It kept crashing on my PC! Every time I placed a new component it went into some auto sim mode?? Unfortunately if you want good results, the time step can't be more than about 10 ns, making it VERY slow. The best you can do is to play with IC on the caps and get the initial start-up transient as smooth as possible.

I attached my setup that I optimized as best I could.

Be patient, it only starts plotting data after the 5 ms mark.

[bobcat1]

Hi
There is a new PSPICE version done specially for TI with free download this software include original simulation modules for all TI chips ,you can use it for accurate simulation
https://www.ti.com/tool/PSPICE-FOR-TI

All the best

Bobi

 

[metal]

there is no UC3843

[optikon]

I have not used MC in the last five or more years. This is not a good tool for SMPS analysis with a switching model. What a frustrating experience. It kept crashing on my PC! Every time I placed a new component it went into some auto sim mode?? Unfortunately if you want good results, the time step can't be more than about 10 ns, making it VERY slow. The best you can do is to play with IC on the caps and get the initial start-up transient as smooth as possible.

I attached my setup that I optimized as best I could.

Be patient, it only starts plotting data after the 5 ms mark.

Yes very true..

Fundamentally, Simetrix and Microcap work the same way for solving transient time steps so I am not sure why you have had a worse experience. Auto sim mode? seems strange.. maybe you should try a recent version?

Techniques like POP should be used when possible.

Its quite common for these spice simulators to reduce the time step to the point of almost an unusable sim time. Has Simetrix been any better for this? I have been thinking about learning it.

[PM3295]

I have downloaded the latest MC. What happens is, when I place or edit a part, it appears to start some sort of massive CPU action. I get the turning circle and CPU use goes max. I have to hit escape and click "exit analysis" every time. It appears it tries to run a new analysis every time I change a value or add a part. Weird.

Simulators running spice models are slow. Simulators running PWL (PSIM is another one) models are super quick, but the models will be very simplistic, so it is a balance. Spice model will not run on a PWL based sim without extracting it from spice. Any complex model extraction like the UC3843 cannot  be done in the UI, so you have to rely on the vendor.
  

Posted on: October 04, 2020, 04:13:09 16:13 - Automerged

there is no UC3843

https://www.ti.com/product/UC3843 spice model can be installed on TINA-TI

[metal]

I see, if you are still in analysis, it will do that, each time you change a component value, you need to make sure you have existed analysis mode. BTW, closing the analysis window where you see graphs is sufficiant to exit analysis mode.

Anyway, I am running the simulation smoothly on Microcap. I need to know if the current thru the inductor is OK this way way or not, see the attachment please.