I've made a LTspice model of a diode bridge rectifier, but when I simulate my circuit, the input voltage is oscillating.

Here is my schematic, along with the simulation result of the voltage at node 3 (marked with an arrow.)

enter image description here

When I zoom in on these weird parts, I can see that it is definitely some kind of oscillation:

enter image description here

I've already tried changing the position of the ground, changing the solver to an alternate solver, and introducing ESR to the capacitor.

The problem seems to be correlated with the capacitor, since when I set a lower capacitance, the output gets better. The output also gets better when I set the capacitor ESR to a few ohms, but that is not very realistic.

I also tried with different diode models, and the problem persists.

Does anyone have an idea what could be the problem?

  • 7
    \$\begingroup\$ 1) Why do you have a 200 uH inductor in the circuit? 2) What happens if you remove the 200 uH inductor? The problem seems to be correlated with the capacitor Resonances like that point to an LC (Inductor, Capacitor) resonance, I only see one inductor and one capacitor in your circuit. \$\endgroup\$ Commented Dec 3, 2021 at 13:12
  • \$\begingroup\$ The node you have picked is not the output of the rectifier - it is the input. The output would normally be take from the junction of D1-D2 and D3-D4. Did you try the plain old 1N4001 diode for your rectifier? \$\endgroup\$
    – JRE
    Commented Dec 3, 2021 at 13:27
  • \$\begingroup\$ @Bimpelrekkie 1) I need that inductor because it models the power supply network that I'm trying to simulate. 2) When I remove it, the problem is gone, so I think you are right - there is probably some resonance between the capacitor and the inductor. I just didn't think that was the case because I also tried using different inductor and capacitor SPICE models, and the result was the same. Thank you, I will see how to avoid that. \$\endgroup\$ Commented Dec 3, 2021 at 13:35
  • \$\begingroup\$ @JRE Yes, you are right, I just didn't express myself correctly - I meant the output of the simulation. I will edit my post to be more clear. I tried with good old 1N4001, but the problem was there, too. \$\endgroup\$ Commented Dec 3, 2021 at 13:36

2 Answers 2


You're getting ringing from the diodes switching off in conjunction with the line inductance (and resonating with the diode capacitance when blocking- maybe 50pF or so). If you add a snubber like 100\$\Omega\$ in series with 47nF across the bridge rectifier input it should go away, mostly or entirely. It's probably unrealistic to have 200uH with zero parallel capacitance as that component of the line impedance but if that is your model, maybe you need to use it.

Frequently, in audio equipment, the diodes are paralleled with a small capacitor to prevent the EMI from showing up as a nasty 100Hz/120Hz buzz in the sound.

  • 2
    \$\begingroup\$ That solved my problem, thank you! Could you tell me where can I learn more about this phenomenon, since I can't find many good references? \$\endgroup\$ Commented Dec 3, 2021 at 14:17
  • 6
    \$\begingroup\$ Try this reference (full text). LC resonance, of course, is basic electronics. \$\endgroup\$ Commented Dec 3, 2021 at 14:19
  • \$\begingroup\$ Why isn't the amplitude the same every half cycle? \$\endgroup\$
    – jy3u4ocy
    Commented Dec 4, 2021 at 12:04
  • 1
    \$\begingroup\$ @jy3u4ocy Excellent question. There are two reasons- the circuit has not reached steady state and it starts off with a positive input. The second, probably more important, reason is that the default time step the SPICE solver uses is a bit large to capture MHz ringing in a tens-of-ms simulation. If you simulate for 150ms and reduce the maximum time step to 50 or 100ns the appearance is very similar for each half cycle. \$\endgroup\$ Commented Dec 4, 2021 at 12:20
  • 2
    \$\begingroup\$ P.S. In situations such as this (with widely varying time scales) you shouldn't expect the amplitude of such high frequencies to be at all accurate unless you tweak the time step. \$\endgroup\$ Commented Dec 4, 2021 at 12:37

When Diodes no longer conduct after the peak sine, diode impedance rapidly rises and the L/ESR or X/R Q factor increases to the point of visible resonance then tapers down as the energy is absorbed by the negative swing conduction of diodes.

It is common to add a small capacitance across each diode,Cd (in addition to the self-capacitance which is maximum at 0V and reduces with negative bias) This will shift the Q and SRF downwards and suppress the EMI by the Cd/1mF ratio. ( aka "Capacitance transformer" works much like an inductive transformer by impedance ratios)

You will find this common on most high-quality audio and TV line full-bridge rectifers.


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.