Inductor Models

How do I design a coupled inductor?

You first (i) draw at least two inductors and then (ii) define the K coefficient between the two inductors. See mutual inductance section.

How do I control the inductor parasitic resistance?

By default, LTspice adds power losses to inductors to aid SMPS transient analysis. For SMPS, these losses are of usually of no consequence, but may be turned off if desired. On the "Tools > Settings > Hacks!" page, uncheck "Supply a min. inductor damping if no Rpar is given" This setting will be remembered between invocations of the program. There is also a default series resistance of 1 milliohm for inductors that aren't mentioned in a mutual inductance statement. This Rser allows LTspice to integrate the inductance as a Norton equivalent circuit instead of Thevenin equivalent in order to reduce the size of the circuit's linearized matrix. If you don't want LTspice to introduce this minimum resistance, you must explicitly set Rser=0 for that inductor. This will require LTspice to use the more cumbersome Thevenin equivalent of the inductor during transient analysis.

How do I add my own inductor model?

Choose File > New Library > Inductor, add inductors, and save the file in Documents/LTspice/user.ind. Do not edit %LOCALAPPDATA%\LTspice\lib\cmp\standard.ind - this file is overwritten when LTspice is updated. However, standard.ind may be opened in LTspice to enable copying inductors to user.ind as a starting point. To use one of the added inductor models, place an inductor on the schematic, right-click, and choose "Select Inductor." This will present a list of all of the inductors in standard.ind as well as those in user.ind.