# How can I model this common mode choke in circuit in LTspice?

How can the common mode choke in below diagram used in LTspice? By an inductor or transformer? How should be the circuit drawn in LTspice?

I want to use this to filter out CM noises for single ended coaxial cable.

• A common mode choke is basically a (1 to 1) transformer and a transformer is basically 2 inductors with mutual coupling. Sep 21, 2017 at 12:18
• Is that correct now for simulation?: i.stack.imgur.com/MhGtX.png Sep 21, 2017 at 12:50
• Yes, that's the idea. I think the orientation of the inductors (where the small circle is) is how it should be but you might want to check that with a simulation. A differential signal should pass through, common mode should be suppressed. Sep 21, 2017 at 12:56
• @floppy380 -- Looks very good, but your K1 spice directive has Lp instead of Lp1, so it should be "K1 Lp1 Ls1 1" in your drawing, though I usually use a lower coupling than 100%. Perhaps "K1 Lp1 Ls1 0.85" would also be more realistic in its coupling proportion? Jan 14, 2021 at 16:14
• You can serach for 'we' in ltspice the you will see the Common mode choke models. Mar 17 at 5:03

At reasonably small currents, a common mode choke looks like a 1:1 transformer with a resistance in parallel with each of its inductors. You can get very close to correct by looking at the impedance vs frequency graph. At low frequencies, the impedance rises like an inductor. Use that to get an inductance value. At some high frequency, the inductance maxes out. Presume your inductance and compute the resistance. This will be good enough for most models.

I would model it with 2 coupled inductors. Here's a pic.

Remember to put the spice directive to couple the inductors

• How do you couple mutually(spice command?) and what will be the values for L1 L2 for a 13mH choke? Sep 21, 2017 at 12:43
• Is that correct now for simulation?: i.stack.imgur.com/MhGtX.png Sep 21, 2017 at 12:51
• K=1 is a way too optimistic. You should check leakage inductance i.e. stray differential on your choke datasheet and lower coupling till you get it. Simulating with zero leakege is very little useful Jan 2, 2018 at 13:24
• @doncarlos I meant Jan 2, 2018 at 13:24
• To set the mutual inductance, point to a blank area, right-click, open the 'Draft' sub-menu, select 'Spice Directive', enter text K1 L1 L2 0.8, left click to place. If you don't want it to be visible, hover over the text, right-click, open pull-down menu 'Justify", scroll up one to '(not visible)'. Jul 14, 2020 at 12:00

Common mode chokes are horribly nonlinear components (impedance varies with frequency and not in an inductance way), good luck modeling them with linear components in spice.

Your schematic seems a whole input filter module so it's even more difficult. In my experience with these things you usually pick the manufacturer diagram and extract the response to work in S-parameter space. And then you build the prototype and nothing works as it should since your chassis maybe has a bend which resonates with an horrible frequency.

Some manufacturers gives you spice modules for some filters. Schurter and Würth comes to mind, look in them to see if there's something similar to your part.