Elien,
Unrelated to your question - Be aware of these things, which might affect your simulation's apparent accuracy:
- Non-coupled inductors in LTspice have a default series resistance of 1 m = 0.001 ohm.? If you want ideal inductors, right-click on each inductor and write "0" for the Series Resistance.
- LTspice uses waveform compression, which is a lossy compression (you can't restore the un-compressed original) but it can significantly reduce the size of the .RAW output file.? All results, including .MEAS command calculations, are affected by that.? If you don't want any impairment from that, disable waveform compression by adding ".options plotwinsize=0" to your schematics.
Footnote about waveform compression:? The .tran command in this simulation specified a Maximum Timestep of 1e-8 = 10 ns.? Yet LTspice compresses the saved waveforms with a larger effective timestep of around 250 ns.? If you really need the timestep to be 10 ns or less, always disable the waveform compression.? Internally, LTspice simulates the circuit with 10 ns or smaller timesteps, but it might not save the simulated waveforms with increments that small, unless you disable the compression.
Andy
