I've been trying to get a Colpitts oscillator to work with multisim, following this schematic, which I found in a book (I just copied it):

Yet, it does not work, all I get is a 0 voltage signal from the oscilloscope.

The same circuit, simulated in LTSpice, worked fine:

enter image description here

So, does anyone with experience in multisim know how to get this simulation to work? A similar oscillator in the "examples -> miscellaneus circuits -> claposcillator" works great, adn the book where I found it also simulated it in Multisim and according to it, simulation works fine as well (book is Electronic devices eighth edition, by Floyd, page 84X)

Here are some of the things I've tried:

  • Add a AC voltage source with low voltage to simulate noise
  • Change the values of the capacitors to the ones in the LTSpice figure
  • Try different transistors and components
  • \$\begingroup\$ Are you sure your 12V connection is actually made? \$\endgroup\$
    – Matt Young
    Commented Jan 29, 2014 at 18:18
  • \$\begingroup\$ Yes.. the error that comes with that red circle is: Error: Connecting Bidirectional to Power: [R3 pin, ....] I've looked it up and it seems to be some sort of Electrical Rules Check setting \$\endgroup\$
    – triplebig
    Commented Jan 29, 2014 at 18:20
  • \$\begingroup\$ Though now that you mentioned it, that same check error doesn't come with the simulations that actually work... hm, I'll look into that right now EDIT: yea, same exact settings, now I'm 100% clueless \$\endgroup\$
    – triplebig
    Commented Jan 29, 2014 at 18:23
  • \$\begingroup\$ For some reason all the resistors and capacitors were "bidirectional". I changed them all to "passive", and there were no errors in the design check. Unfortunately, the same problem ensued... \$\endgroup\$
    – triplebig
    Commented Jan 29, 2014 at 18:48

2 Answers 2


It's not the same circuit on the emitter. You've got a 1k pot in series with a 1k resistor and the pot wiper connects to a grounding capacitor. You've also got a 10pF cap where it is 100nF in LTSpice.

I'm not saying any of these matter but you can't possibly make comparisons with these glaring disparities.


Following comments from the OP, the problem I think arises from the new "intended" operating frequency of the circuit (he uses a 10pF cap on the multisim circuit to set the resonant frequency whilst the LTSpice circuit has 100nF). Added to this is the lack of emitter capacitor - the multisim circuit shows it connected via the wiper of a pot set midway and this will drastically reduce the gain and prevent or delay oscillation. Remember that the collector has to generate enough signal to drive the 10nF capacitor (C3) and at a much higher frequency this 10nF (via C5, 1uF) will probably look like a short circuit - the gain of the transistor has to be greater than 1 for it to begin oscillation and with no directly connected emitter capacitor and a 10nF effectively connected to the collector I think the gain will be less than unity.

I'm not totally familiar with this type of Colpitts oscillator but it seems to me that the LTSpice circuit should oscillate at about 41kHz whereas the MS circuit should operate at about 4.1MHz - this isn't going to happen with a 10pF - its reactance at 4.1MHz will be nearly 4 kohms and this will get "battered" by R1 and R2 in the imedance versus resistance race. Do the sensible thing and start with the same circuit. On the LT circuit, the 100nF will have an impedance of about 40 ohms at 41kHz and therefore not be hardly affected by R1 and R2.

  • \$\begingroup\$ I didn't change them because they should still give me an oscillation, but with different frequencies and gain. In any case, to be sure, I've changed the circuit to exactly the one in LTSpice, and the same problem occurred \$\endgroup\$
    – triplebig
    Commented Jan 29, 2014 at 18:39
  • \$\begingroup\$ have you tried letting the circuit run for up to a second just to check that it definitely doesn't oscillate after a few hundred milliseconds. Colpitts can be slow starters and I've hit this problem on my simulator. \$\endgroup\$
    – Andy aka
    Commented Jan 29, 2014 at 19:14
  • 1
    \$\begingroup\$ I'd also make the component values the same because that 10pF cap may prefer having lighter base bias resistors. Make the emitter the same too because at the moment, your gain will be drastically reduced with the wiper set central. \$\endgroup\$
    – Andy aka
    Commented Jan 29, 2014 at 19:18
  • \$\begingroup\$ So I got it to work, and that I had to: 1) Set a lower time-step, for some reason the automatic one didn't help 2) Remove the potentiometer. It's funny that I found this in a book, and I triple-checked that it's exctly like the book schematic. When I redid the circuit it still didn't work because 3) It "still had a "bidirectional" capacitor instead of a "passive one"(whatever that means..), so I had to replace it. Lot's of things going wrong but at least I see the blessed sine wave. \$\endgroup\$
    – triplebig
    Commented Jan 29, 2014 at 19:45
  • \$\begingroup\$ The osc frequency seen is 130khz.. if you substitute into the colpitts formula you get 137kHz, so it seems close enough. Could you explain why the gain is drastically reduced with the pot? I'm having a bit of trouble understanding this \$\endgroup\$
    – triplebig
    Commented Jan 29, 2014 at 19:53

I had the same problem in past. Try other transistor. Adjust Time Step (low values). Make capacitors and inductors have any initial value.


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.