I'm on a quest to simulate various circuits in LTspice that are a part of an Elenco project kit. All has been going well until I started trying to simulate some simple oscillator circuits.

In the project you close a switch to turn on the +9VDC from a battery to start the oscillator which I'm simulating by using a pulse. I should be seeing a roughly 2Hz oscillation going though the LED while the 9V is applied, but it isn't working in LTSpice. Text Text

The inductors are from the primary side of a transformer. The project booklet gave the values of 300mH from one end to the other with a center tap that divides the inductance in half. I measured a series resistance through each inductor of around 90 ohms so I added that in case it would help. I'm not sure exactly what types of LEDs or transistors they used in the project. At the very least I know the transistor is a BPJ NPN.

Link to the .asc https://github.com/mmprkdev/LTspice/blob/main/Oscillator.asc


  • 4
    \$\begingroup\$ Joule thieves rely on saturation of the magnetic core which you didn't simulate. \$\endgroup\$
    – Andy aka
    Commented Feb 9, 2022 at 20:36
  • 7
    \$\begingroup\$ Also, if L1 and L2 are on the same core, then LTspice needs to be told these are coupled. Add a K1 L1 L2 0.99 operation (.op button) to the schematic. \$\endgroup\$
    – rdtsc
    Commented Feb 9, 2022 at 20:43

1 Answer 1


You need a coupling factor between the coils. Add spice directive K L1 L2 0.99 (or a similar coupling factor slightly less than 1).

C1 is too large. Reduce it to ~8 μF.

  • \$\begingroup\$ Thanks, I didn't realize I had to couple those inductors. \$\endgroup\$
    – aj-10
    Commented Feb 10, 2022 at 19:01
  • \$\begingroup\$ Is it normal to see those spikes of -3kV for each oscillation on the base of the transistor? \$\endgroup\$
    – aj-10
    Commented Feb 10, 2022 at 19:28
  • \$\begingroup\$ Yes, it's normal to see such anomalies in LTspice, because most transistor models don't include the Base-Emitter reverse breakdown characteristic. You can simulate it with a diode and 6.8V zener wired in series to limit reverse voltage to ~-7.5V. For more realistic results you should also add inductor core loss (simulate it with parallel resistance) and capacitance. \$\endgroup\$ Commented Feb 11, 2022 at 3:36

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.