7
\$\begingroup\$

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?

enter image description here

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

enter image description here

\$\endgroup\$
4
  • 2
    \$\begingroup\$ A common mode choke is basically a (1 to 1) transformer and a transformer is basically 2 inductors with mutual coupling. \$\endgroup\$ – Bimpelrekkie Sep 21 '17 at 12:18
  • \$\begingroup\$ Is that correct now for simulation?: i.stack.imgur.com/MhGtX.png \$\endgroup\$ – floppy380 Sep 21 '17 at 12:50
  • \$\begingroup\$ 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. \$\endgroup\$ – Bimpelrekkie Sep 21 '17 at 12:56
  • \$\begingroup\$ @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? \$\endgroup\$ – MicroservicesOnDDD Jan 14 at 16:14
1
\$\begingroup\$

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.

\$\endgroup\$
0
\$\begingroup\$

I would model it with 2 coupled inductors. Here's a pic.enter image description here

Remember to put the spice directive to couple the inductors

\$\endgroup\$
6
  • 1
    \$\begingroup\$ How do you couple mutually(spice command?) and what will be the values for L1 L2 for a 13mH choke? \$\endgroup\$ – floppy380 Sep 21 '17 at 12:43
  • \$\begingroup\$ Is that correct now for simulation?: i.stack.imgur.com/MhGtX.png \$\endgroup\$ – floppy380 Sep 21 '17 at 12:51
  • \$\begingroup\$ 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 \$\endgroup\$ – carloc Jan 2 '18 at 13:24
  • \$\begingroup\$ @doncarlos I meant \$\endgroup\$ – carloc Jan 2 '18 at 13:24
  • 1
    \$\begingroup\$ 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)'. \$\endgroup\$ – Mike Bushroe Jul 14 '20 at 12:00
0
\$\begingroup\$

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.

\$\endgroup\$

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.