Average Current Mode Boost Converter

Thread Starter

joshi65201

Joined Sep 4, 2015
14
I have designed boost converter with the average current mode compensation using the example in "Designing Stable Control Loops By Dan Mitchell and Bob Mammano" but not getting the correct output.Attaching the Ltspice schematic,please advise where I went wrong.I have used the same schematic with same component values in the example. Please save the attachment with .asc extension and then open in LTspice.

Thanks
 

Attachments

Thread Starter

joshi65201

Joined Sep 4, 2015
14
Its working on my laptop,I tried simulating the schematic once again and it Worked .Here's the screenshot of the results and Boost Schematic for your reference.

Boost_avg_current_mode.png schematic.png
 

eeabe

Joined Nov 30, 2013
59
I got it to run, and here are some issues I found:

1) The +5V supply was not labeled the same as the +5V net label on the LT1002A, so it was not powered.
2) The default NMOS you are using to switch doesn't seem to get turned on with the 4V output of U4. Try a real mosfet model. (Right click on it and click on Pick New MOSFET.)
3) The output of op amp U5 seems to be so low that U4 gets set on constantly instead of toggling. The LT1002 doesn't have a rail to rail input range. Maybe an op-amp with a common mode range that extends to or beyond ground would help.

Maybe that will help you get a little further.
 

crutschow

Joined Mar 14, 2008
24,039
Your circuit is not working, at least not as a switching regulator to give you the boosted 16V or so the reference voltage component values (5V, R3 and R4) would imply. The output you see is simply the 12V from V1.

For starters, U1 needs to be a fast comparator (labeled Comp in the Fig. 33 your reference schematic) to switch at the 100kHz switching frequency you are using, not the slow LT1002A op amp you have in the schematic.
As a side note, 1k is likely too high a value for R8 to generate a good 100kHz square-wave to the high gate capacitance of M1 (which needs a part value).

Also, if you look carefully at Fig. 33 you will see that the "connection" circle to the drain of M1 is a current transformer (as noted in the write-up which you read I assume(?)).
Alternately you could add a small resistor in series with the source of M1 to give a voltage proportional to the current but that would reduce efficiency, of course.

There may be other problems, but those two jumped out at me at first glance.

Note that you can post .asc Ltspice files directly to this forum. You don't need to convert them to .txt.
 
Last edited:

Thread Starter

joshi65201

Joined Sep 4, 2015
14
Thanks so much for all your prompt responses,I have altered the schematic as per the suggestions but now simulations is taking ages to complete.

@crutschow : connection circle to the drain of M1 is a current transformer,I looked into it and though they might be sensing both on and off state current through common current sense resistor(Rs). But now i have changed it to the current controlled current sources.I am attaching the updated schematic.Please advise any suitable method to fasten the simulations.I tried replacing NMOS with switch,but doesn't help much.
 

Attachments

crutschow

Joined Mar 14, 2008
24,039
As I previously noted, an op amp is much too slow for U4.
It needs to be a high speed comparator.

Also your feedback loop appears to have positive feedback. Try reversing the inputs to U4.

Simulations of switching regulators generally take a long time due to the long time-constants involved for the inductor and output capacitor along with the high switching frequency. That means you have to simulate the switching of thousands of clock cycles before the output settles to a steady output.
Doing an initial condition Spice Directive of .ic v(out) =12V can help speed the startup where v(out) is the output node.
(Note that it helps to label all the nodes of interest with labels such as in or out using the "Label Net" F4 command.)

To get the circuit operating initially I suggest you remove all parts of the current feedback loop and just try to get the voltage feedback portion working.
After that you can then try re-introducing the current feedback loop.
 

Thread Starter

joshi65201

Joined Sep 4, 2015
14
@Alec_t & @crutschow :Thanks for your responses.My Apologies with current transformer( ratio should be .01 instead of 100) and simulation speed increases.

I have changed op-amp U6 to LT1226 having GBW=1Ghz and 400v/us slew rate.
For positive feedback, I have one inverting amplifier and two non-inverting amplifier in the feedback path as per previous configuration,hence shouldn't that be negative feedback.
Problem, I am facing now is output is 20v but not 24v(for which the schematic is designed). However if I put the spice directive ".ic v(output)=12V", output drops to 11.48v(I didn't understand..why..?).I am attaching the updated schematic with simulation results.

Output of the op-amp U1 is few mV , but Boost Converter keeps its output voltage stable at 20v even if I change the input voltage to 13v, 15v,18v.Hence feedback is working but just need to get correct output voltage.

Also, Please advise while implementing in actual hardware, how can we realize the current transformer.
Boost.png
 

Attachments

crutschow

Joined Mar 14, 2008
24,039
Why do you insist on using an op amp for U6, when I stated twice that you need to use a high speed comparator?
Try an LT1720 instead, for example.
Also there seems to be a problem with the LT1014D op amp model.
Try an LT1366 or LT1498 for U1 and U2.

With those comparator and op amp changes, the output settles to 16.8V which is close to the 16.7V as calculated from the values of R3 and R4. (Don't know how you got 24V for that(?))

Edit: I also had to change the sawtooth output of V2 from 0V-2V to 2V-4V amplitude to get proper operation.
Below is the modified circuit with R3 = 16.1k to give 24V output.
 

Attachments

Last edited:

Thread Starter

joshi65201

Joined Sep 4, 2015
14
@crutschow :This forum is awesome,Loads of thanks for your prompt responses, I figured out that I messed with R3 calculations from your previous post and start getting the correct output.Thanks again for posting the updated schematic.I will try to do the AC simulations now for check for the Phase margin and other stability parameters and will get back in case of questions.
 

Thread Starter

joshi65201

Joined Sep 4, 2015
14
@crutschow : Any idea how to do the AC analysis with the boost converter,I have changed the switching element with DC transformer,but seems not working.Regarding the turn ratio,I figured out value 4 probing at the node voltages in the schematic.I am attaching the schematic,I used for the AC analysis.
 

Attachments

crutschow

Joined Mar 14, 2008
24,039
LTspice does not do an AC analysis of a switching circuit.
It can only do AC analysis of linear analog models.
So if you want to do an AC analysis you will need to substitute linear models for all the switching elements.
I've done that for a buck regulator but not sure how to do it for a boost regulator.
You should be able to find some info here on how to make the conversion.
 

Thread Starter

joshi65201

Joined Sep 4, 2015
14
I have tried AC simulations for the Boost converter replacing all the non-linear switching elements with their average models.Attached is the screenshot for the schematic and Average switching model for the Boost converter and Gain and Phase plots obtained.However they doesn't seem to match with the Plots given in the design documents.Please chip in your thoughts.

Symbol.PNG Boost_Average_Model.PNG Boost_Feedback.PNG Staibility_Plots.PNG
 
Last edited:

crutschow

Joined Mar 14, 2008
24,039
You still have X1, which appears to be a switch, in your circuit.
Switches are non-linear and won't AC simulate.
 
Last edited:

Thread Starter

joshi65201

Joined Sep 4, 2015
14
X1 as in symbol looks like switch,it back schematic is Boost_Average_Model.PNG which is the average model.Just resemble actual hardware,I made look similar to the components we have in the Boost converter for the ease of placement.
 

Thread Starter

joshi65201

Joined Sep 4, 2015
14
Also, please advise how can I implement the current sense.I am thinking to use the series resistor in series with the source of the switching device and hall sensor to sense the diode current and summing amplifier to add the sense voltages.Please advise, if you have more viable solution to this.
 

Thread Starter

joshi65201

Joined Sep 4, 2015
14
Hi,
I also tried designing the boost converter using the voltage mode compensation in matlab and designed the circuit in LTspice,however I am not getting the correct output(should be 20v) but getting 48v and that too vary with the input voltage.Please advise where I went wrong.

Thanks in advance
 

Attachments

Top