I was simulating this simple boost converter circuit in LTSpice and it always gives an incorrect output voltage. (Almost 500V, compared to 444V obtained by calculation).


As the IRF430 model is not available in the software, I tried using the model given in Infineon website, producing the following plot for output voltage. Output voltage plot using manufacturer's model Then I tried the simulation replacing the model with one given in a book which produced the following result. Output when using a different model

Then I simulated the same circuit in Cadence PSpice using same parameters, and surprisingly it produced an output waveform similar to the second result with the final stable output at ~444V. Was I doing something wrong in LTSpice or can this be considered a bug in the software?

  • 5
    \$\begingroup\$ You need to set the rise and fall time in LTspice. I set 1ns and Vout = 444V. Because the LTspice automatically will use a default value for <trise> and <tfall> if these parameters are set to zero. Default value: 10% of Ton or 10% of Tperiod-Ton whatever is smaller. You must specify Trise and Tfall if you want a certain value. \$\endgroup\$
    – G36
    Commented May 7, 2017 at 10:56
  • \$\begingroup\$ Thank you! This worked. I used to set 1ns rise/fall out of habit for these frequencies but this time I was following a tutorial. I guess my lecturer focused on PSpice only and it somehow defaulted the value to a more appropriate one. \$\endgroup\$
    – chamod
    Commented May 7, 2017 at 13:03
  • \$\begingroup\$ Suggest you update your latest copy of LTSpice as you don't know what restrictions will be placed upon it by Analogue Devices in the future... \$\endgroup\$
    – Paul Uszak
    Commented May 7, 2017 at 23:07
  • \$\begingroup\$ It's very safe to assume LTspice shows the correct results based on the input. In other words, garbage in, garbage out. \$\endgroup\$ Commented May 9, 2017 at 6:12
  • \$\begingroup\$ I would recommend to add parasitic elements in series with L and C, rL and rC. These elements have damping effects and will help the simulator converge. Please also note that if the dc transfer function of the perfect boost is Vout = Vin x 1/(1-D) adding parasitic terms - like the MOSFET rDS(on) - will change this equation and reduces Vout. However, if with a 500-V output, the diode Vf is of less importance, adding these series terms will let you know if the boost ratio you want has a physical sense or not (see latch-up phenomenon of the boost converter). \$\endgroup\$ Commented May 12, 2017 at 11:02

1 Answer 1


You can only consider this half an answer, but might help to focus your efforts nevertheless. It's highly unlikely that such a simple circuit would fall upon a bug in LTSpice. Linear Technology (now Analogue Devices) set their stall out with this simulation package, and their reputation. They market much more complicated DC converters and high precision amplifiers with associated LTSpice models which all perform flawlessly. The tool is used throughout the world by tens of people. Every time I use it and the result is wrong, I eventually find that it was me all along.

We've not seen your custom library files, but I might look towards the pulse definition. 0 12 0 0 0 means zero rise and fall times which is a little unrealistic. Have you looked at the FET drive current that's being simulated? That might be overly high as the source is an unrealistic zero impedance. I think that you have to accept with a very high confidence that in this simple case, LTSpice is probably right based on the models you've input.

Being human, Kazimierczuk and Ayachit could be slightly wrong.

  • \$\begingroup\$ I also found the FET drive unusually high. It contributed to high spikes on the output as well. But as you suspected the problem has been in the pulse definition. \$\endgroup\$
    – chamod
    Commented May 7, 2017 at 13:09
  • 1
    \$\begingroup\$ "The tool is used throughout the world by tens of people." I hope it's a bit more than that! \$\endgroup\$
    – pipe
    Commented May 8, 2017 at 4:48

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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