There seems to be a few questions around this but none of the suggestions solved the issue for me. I apologize for the long question but I would like to present my thinking and everything I tried.

Mostly as an exercise, I set off to build Common Emitter Colpitts oscillator, following this nice, in-depth app note.

I understand that oscillation will occur when:

  1. The loop gain magnitude is at least \$1\$
  2. The loop gain phase is \$ 2k\pi \$

So I started by simulating and building a CE amplifier: enter image description here

So I did some math and got the following operating point:

  • Base voltage \$V_B = 1.24V \$
  • Emitter voltage \$V_E = 0.54V \$
  • Collector voltage \$ V_C = 2.7V \$
  • Collector current \$I_C = 1.15mA \$ Furthermore:
  • The gain is approximately (neglecting \$R_5 >> R_3\$) \$A_V = -4.26\$. This provides a phase shift \$\pi\$ and therefore the feedback network needs to add \$\pi\$ as well.

SPICE seems to agree with the above numbers on the operating point and gain.

Therefore I went ahead and focused on the feedback network: enter image description here

  • \$V_1, R_3\$ are the Thevenin equivalent of the \$Q_1\$ output current source with \$R_3\$ in parallel
  • \$D_1, D_2\$ provide some gain control to avoid the collector waveform clashing with the emitter waveform. \$C_2\$ capacitively couples the signal so that the collector bias point is not shorted to ground through the diodes
  • The CLC filter has unitary gain at the design frequency of approximately \$2.2MHz\$ and a [hase shift of \$\pi\$
  • \$ C_1, R_{beq}\$ are the CE stage input capacitor and the base biasing network equivalent resistor (neglecting the impedance looking into the base which is approx \$100k\$)

I simulated the whole filter and the attenuation is approximately \$5dB\$ at the design frequency.However, this should be compensated by the CE stage gain. enter image description here

Everything looked good on paper so I breadboarded it and it does not oscillate.

enter image description here A few more notes:

  • The inductor has a SRF of at least \$60MHz\$ so I am confident it is not self-resonating
  • I tried several values of \$C_1\$ and \$C_2\$ around the values in the schematic
  • I tried reducing \$R_4\$ to increase the gain, as I thought that maybe the real-world attenuation is bigger than I expect (especially on breadboard)
  • The power-supply is decoupled with $\100nF$

Below is my setup. The top and bottom positive and negative rails are connected at the other end of the breadboard. enter image description here

I would really appreciate any input on what to do to debug this. Thanks

  • \$\begingroup\$ Looks like a capacitor (yellow) connects transistor collector-to-emitter that shouldn't be there. Also, do you have the top ground rail connected to the bottom ground rail? \$\endgroup\$
    – glen_geek
    Commented Jun 13, 2021 at 12:39
  • \$\begingroup\$ Have you characterized that (suspect) inductor at 2.2 MHz? To get oscillations, even under ideal SPICE simulation, its Q must be greater than about 80. It's quality is likely not quite so high. \$\endgroup\$
    – glen_geek
    Commented Jun 13, 2021 at 13:02
  • \$\begingroup\$ The capacitor connecting emitter to collector wasn't there originally. I tried adding it as I followed a recommendation found in a similar answer. \$\endgroup\$
    – jack
    Commented Jun 13, 2021 at 13:12
  • \$\begingroup\$ The inductor is a suspect and I agree. It's from CPC TF00567 but the picture there looks very different from the part I got. I'll try that and feed back. \$\endgroup\$
    – jack
    Commented Jun 13, 2021 at 13:13
  • \$\begingroup\$ Yes, the top and bottom rails are connected at the other end of the breadboard. \$\endgroup\$
    – jack
    Commented Jun 13, 2021 at 13:13

1 Answer 1


This looks like an exercise in determining what influences an oscillator where it is barely oscillating. An excellent treatment of threshold oscillations is found in Introduction to Radio Frequency Design by W.H.Hayward.

Component quality and their stray reactances, resistances should be included - a SPICE simulation often gives optimistic results because these are not added to a simulation. In this example, transistor characteristics which might vary significantly from device-to-device are swamped by that unbypassed emitter resistor.
An inductor is often the component having less-than-ideal characteristics. In the simulation below, its internal resistance is simplified to a series resistor, which was varied in value until oscillations were achieved...anything above 1 ohm killed oscillation. Its self-resonant frequency was accommodated by a bulk, parallel capacitor of 2.06pf.
The breadboard photo suggested that a significant missing capacitance exists between collector and base, which are on adjacent breadboard strips. A measurement on a similar-looking breadboard showed about 6pf. I've added a few more pf for stray-coupling.
There are other wiring reactances not added to the simulation, like the inductance of the long ground path from breadboard top-to-bottom. Is this significant? Perhaps not at 2.2 MHz.

To test oscillation threshold in AC analysis, I added an AC current source to transistor base (not shown below): extra components added to spice model
With inductor's resistance set to one ohm, oscillation was barely achieved at 2.24MHz. This corresponds to an inductor Q of 140. If the inductor spec sheet says Q is minimum of 70 at 2.52 MHz, you most likely don't have an oscillator.

Why consider any more component's quality or strays when the inductor quality already kills oscillation? I'd welcome any suggestions as to other significant (missing) oscillation-killers.

  • \$\begingroup\$ Thanks @glen_geek, that really helps. I’ll pay more attention to inductor Q when procuring an alternative. \$\endgroup\$
    – jack
    Commented Jun 13, 2021 at 15:24

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.