My goal is to understand and design a class E power oscillator. To this end, I am trying simulate the following schematic using LTSpice. Circuit topology and the design values are extracted from the paper "from here" -

design specifications used in the paper are; Pout =1W, Supply =4.5V, frequency 800kHz, RL=50ohm, QL=13, efficiency =90% Objective of this question is not to understand the paper, but to understand why my repeat simulations does not work - of course, I believe that the circuit should work fine with their values. But to make the question clearer, in this paper, the circuit is modeled using its equivalent impedance sections (assuming only the fundamental harmonic) and the component values are calculated by using class E design equations for 0.5 duty. Few things to note: In their analysis, the the gate-to-source impedance of the MOSFET, Zgs was measured at 800 kHz and used for the analytical equations, and voltage divider is experimentally tuned to obtain 0.5 duty.

(differences from the original paper are 1. make R2 170k -> 150k because it was not producing the oscillation when R2=170k, 2. zener diode model was not given in the paper)

enter image description here

However, I the oscillation waveforms are follows. Which include Drain Voltage - V(D); Gate voltage - V(G), Voltage across RL - V(RL+) and supply current - I(V1) enter image description here

What could be the reason for this oscillator not working as expected? (It is expected to deliver approximately 1W power to RL, but here it is only few milliwatts)

Alternatively, can someone suggest any other reference (preferably open access) to design a class E power oscillator close tho the same design specs?

  • \$\begingroup\$ You can only view the original if you are an IEEE member. Are you wishing answers to be restricted to those people? Mark the nodes you measured on your schematic too. \$\endgroup\$
    – Andy aka
    May 17, 2018 at 12:14
  • 1
    \$\begingroup\$ Looks like the first job is to find the LF resonance and kill it. What does the paper say about L3 and Cgs/Cgd? \$\endgroup\$
    – user16324
    May 17, 2018 at 12:34
  • \$\begingroup\$ Andy if you copy the IEEE title, you can locate elsewhere (sometimes) \$\endgroup\$ May 17, 2018 at 12:35
  • 1
    \$\begingroup\$ C3 and Cbp are uselss. If you want them to be active, impose 4.5 Rser=10m (for example) in V1. Better yet, make it 4.5 Rser=10m Cpar=1u. \$\endgroup\$ May 17, 2018 at 12:59
  • 1
    \$\begingroup\$ Whenever I see paper with reactive parts that use 4 digit values, I expect the design to overlook many sources of error. This osc must have enough gm or gain to overcome the C ratio attenuator. You have a 71kHz Osc. I wonder what your layout looks like \$\endgroup\$ May 17, 2018 at 13:06

1 Answer 1


I see the inductors are showing the dot, that's usually if there is some coupling (unless manually shown). Here's my attempt, no coupling:


and some details for the waveforms as in your example. Note that V(x) is V(RL+), and I used parasitics for the supply, which means the current through it incorporates what would have been your capacitors (if you had some resistance between the supply and the caps, as per the comment):


  • \$\begingroup\$ Thanks, Now I have a working circuit for further study. But when I used mosfet model MTP3055 (downloaded from link), it was still not oscillating. not sure if it is due to the parasitic or issue with the model - anyway, it doesn't matter much now. Roger your comment. Next is to go one step further into efficiency analysis! \$\endgroup\$
    – Pojj
    May 17, 2018 at 14:24
  • \$\begingroup\$ There is a much better topology and do you have any efficiency target? \$\endgroup\$ May 17, 2018 at 14:46
  • 1
    \$\begingroup\$ @Pojj Those are subcircuits (i.e. more involved models), so I can't tell you what's wrong or not, I simply used a .model from LTspice's database. But I'd advise using different MOSFETs, even IRF has made newer, better ones than those, they're pretty ancient. \$\endgroup\$ May 17, 2018 at 14:56
  • 1
    \$\begingroup\$ @Pojj For this setup, it looks like a 100~300mOhm Rdson would be the choice, the gate charge is not so much of concern. If you want higher power, then raising Rdson is not a sensible choice. Also, the Vds seems too high, since the drain voltage is ~3x the supply (maybe higher with different topologies), but the current is what you're after, for power. You could easily make an olscillator with kV on the drain, but almost no current. Power needs current, so lower Rdson, but not too low or it may damp the oscillations, instead. \$\endgroup\$ May 17, 2018 at 15:24
  • 1
    \$\begingroup\$ @Pojj The MOSFET capacitances come into play when choosing the values for the inductances and capacitances. Small or large, they'll influence mostly numerically, since you don't have here hard switching to account for transtion losses. Still, you don't want them too high (e.g. too many nF, or even tens of nF), since those will account for dissipation. And too low (hundreds or tens of pF) will cause fewer losses, but probably generate higher values for Ls and smaller for Cs, thus higher Q, thus higher instability (analog elements do suffer from it). In short, difficult to say. \$\endgroup\$ May 17, 2018 at 16:09

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.