1
\$\begingroup\$

I am designing a product which uses the LTC3122 as a 5V-12V boost converter (datasheet here). This particular device provides the ability to add gain compensation, phase lead, or both. In my case I am only using the gain compensation network, as seen in the image below:

enter image description here

R13 and C28 form the phase lead network (marked as "DNP" in my case since they are not populated), and R12 and C26 form the gain compensation network.

I calculated these values based on the requirements for my project, and now I would like to illustrate the effect that adding the compensation has on the output of the system. I want to do this by generating two Bode plots - one for the circuit with R12 and C26 included and one without. However, I seem to be having some difficulty generating these Bode plots. I attempted to perform an AC simulation of the design in LTSpice but received a warning saying that "This simulation calls a time-domain model...", effectively saying that the simulation would be pointless. I then tried following the process described in this link to obtain a Bode plot, but the simulation has been running for hours and still has not completed. The status bar at the bottom of the LTSpice window says it is 0.3% complete after running for almost four hours. I don't expect it will be able to find a solution. Below is an image of the LTSpice schematic pane:

enter image description here

What other methods could I use to obtain the Bode plot(s) for this boost converter? I went through the datasheet and, while it contains a large number of equations and formulas for poles and zeros, I'm still not convinced I have enough information to determine the full closed-loop transfer function of the model. I would greatly appreciate some assistance from someone more experienced with LTSpice and/or obtaining Bode plots of boost converters than I am. I am basically looking for a Bode plot like the one shown on Page 17 of the datasheet (below), but I want to be able to generate my own so that I can show a side-by-side illustrating the differences between the responses of the compensated vs. uncompensated systems.

enter image description here

\$\endgroup\$
  • 1
    \$\begingroup\$ I corrected a typo in your title. Or, there really is something called a "Boos converter", and I've just made a horrible mistake. \$\endgroup\$ – TimWescott Apr 16 at 20:25
  • \$\begingroup\$ Have you looked at the examples provided by LTspice in the examples\FRA folder? \$\endgroup\$ – jonk Apr 16 at 20:42
  • \$\begingroup\$ You can have a look at this seminar cbasso.pagesperso-orange.fr/Downloads/PPTs/… where I present different ways to obtain the control-to-output transfer function of the boost converter and what compensation strategy to apply. \$\endgroup\$ – Verbal Kint Apr 16 at 20:43
3
\$\begingroup\$

You probably already know this but I'll provide it for users who may not know about it. LT power cad can be useful for checking compensation and it generates bode plots and most all of the linear DC to DC converters are available for checking. It also does a handy power calculation for most converters.

It also does parastics.

enter image description here

enter image description here

enter image description here

\$\endgroup\$
  • 1
    \$\begingroup\$ This is an awesome tool! I didn't even know it existed! Unfortunately it keeps hanging when I click on the Loop Comp. & Load Transient tab after entering my own values. It worked when I used the reference design. It's a long shot, but do you have any idea what might cause it to hang when I enter my own values? The values I entered are the ones shown in the schematic(s) in my original question. \$\endgroup\$ – DerStrom8 Apr 17 at 11:19
  • \$\begingroup\$ UPDATE: I decided to simply enter the component values and forget about selecting specific models for the passives, and it seems to be working now. Thanks very much for the help! \$\endgroup\$ – DerStrom8 Apr 17 at 11:34
  • \$\begingroup\$ I was going the LT spice route and then I found powercad, It's very useful, glad you got it working \$\endgroup\$ – laptop2d Apr 17 at 15:11
2
\$\begingroup\$

You're running into the typical problem of trying to get a frequency response from a transient model. The switching time is much shorter than the loop bandwidth meaning you need to run a huge number of switching cycles at small simulation time steps to get meaningful results.

Here are your options:

  1. Get a much faster computer and let the transient simulation you linked run until finished.

  2. Find out if LT has an averaged model for the converter, use that instead. (Preferred option)

  3. Develop your own averaged model, maybe with the help of the LT technical support staff as needed. The PWM switch model works well for this. Use this in LTSPICE or MATLAB/MATHCAD to generate the Bode plots.

  4. Find out if a SIMPLIS model exists. SIMPLIS is a transient simulator that runs fast enough to generate bode plots from transient models. I think there's a limited free version you could use.

  5. Build the actual hardware, use a frequency response analyzer to measure the loop response.

  6. Just use step response to evaluate stability (in simulation or hardware). When the step response looks good your compensation is likely fine. You can see the effects of changing the compensation in the settling time (or lack thereof) in the step response.

\$\endgroup\$
  • 1
    \$\begingroup\$ A caveat on step responses: it's a good idea to try it on different sized steps, until you get responses that are the same shape. That'll let you explore a good part of the nonlinear range of the thing, as well as letting you know when it starts to behave as a linear system. \$\endgroup\$ – TimWescott Apr 16 at 20:23
  • \$\begingroup\$ @TimWescott excellent advise, I agree completely. \$\endgroup\$ – John D Apr 16 at 21:17
-3
\$\begingroup\$

I find all of Falstad's Physics Tools best for solving simple questions. Choosing the right model for each non-ideal part is what I do. This is especially useful when models for parts are not available, so you emulate the datasheet response then do "what if" mods for ESR or stray coupling.

There are 3 main sub-sites for; 1)Fourier waves, 2) Bode Plots and filters, interactive time 3) scope analysis. Going between (2) and (3) is possible by exporting data & importing on other site for some things.

It takes some imagination and learning the keyboard commands ( like "r" to draw a resistor, "c" a cap., but worth it.

Then any part can be added, edited or even add an ideal switch at 1GHz to compare stripline filters A vs B.

The cursor shows the reading of amplitude and phase ( options)

e.g. enter image description here

Here more phase lead is added after 30kHz where it does not in the lower version.

\$\endgroup\$
  • \$\begingroup\$ If you can imagine it, you can simulate it otherwise you can vote -1 for no imagination \$\endgroup\$ – Sunnyskyguy EE75 Apr 16 at 21:08
  • \$\begingroup\$ I can't imagine falstad simulating the inner workings of an LTC3122 \$\endgroup\$ – laptop2d Apr 16 at 22:05
  • \$\begingroup\$ You need to simulate the external part variations to examine sensitivity to phase margin here to overshoot, load regulation error from any matching starting point, but with effort one could simulate it , if known, but it isn’t. The key to any design breaking down the interface to smaller sections, with an overall concept such as Verbal’s link \$\endgroup\$ – Sunnyskyguy EE75 Apr 16 at 22:29

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.