colpitts oscillator not working

[triplebig]

Hello,

This circuit is exactly like the one in page 830 of the book " Electronic Devices" Eighth Edition by Floyd. I've triplechecked that I have the same circuit in multisim, but I still don't get the circuit to oscillate. 

Can anyone please help? I've spent hours already with this... Here's the circuit:

When I click on the osciloscope, I get a 0V reading, no matter what. DC characteristics look fine. Attached is the file I'm using.

Thanks in advance!

[johnsold]

Oscillators can be difficult to simulate because many require the presence of noise or some random fluctuation to get the oscillation started. The simulation typically does not have that boost.  Sometimes you can get them to start by applying an initial condition to a capacitor or inductor which is different from the steady state condition. Other issues include the time it takes for the oscillation to start and the timestep size in the simulation. All oscillators have some kind of non-linearity which limits the amplitude of the oscillation. Depending on the details of the model for Q1, the non-linearities may not be included at all or may not be very representative of the performance of a real transistor.

The nodes connecting C5-C3-L2 and C1-C4-L2 do not have DC paths to ground. Some simulators can have problems with nodes like that. I do not have Multisim, so I cannot comment on how it handles such cases.

Lynn

[triplebig]

Hello john, and thanks for your response.

Since your post I've tried adding a small AC source, to simulate noise, and that didn't work out. I've also added a 20k resistor to ground to give the DC path you suggested, also, nothing. The thing is, I'm getting a signal that's ZERO in all of those cases, even with a 0.1V ac source between C1 and C4/L2. Only when I add a ground directly to the C5 capacitor do I get a steady DC voltage on the oscilloscpe (2 Volts I think) 

This sounds like this is a software/settings issue, because: 

1) The circuit is exactly like the one in the book, which has a graph with the oscillations, and is using multisim. 

2) For reference, I also found that the example circuit ClappOscillator.ms13 works fine as well, and it is very similar:

3) AND, if that were not reason enough to despair, I tried simulating it on LTSpice and it worked fine, without much hassle, the same exact circuit.

So I really don't know what's going on here and am disappointed that I'm having so much trouble getting a simple oscillator to work. 

[Tien_P]

Hi Triplebig,

I agree with what Lynn said about oscillator circuits, they are very difficult to simulate in a SPICE environment.  However, since you were able to get the circuit to run in LTspice, it should likely work in Multisim as well. In the original circuit you posted, you used rated resistors, capacitors and inductors; I suggest you avoid using these type of components in general. In the component browser under the Basic group, there are RLC families, pick the parts from these families instead.

If you can post the LTspice netlist, I will import it into Multisim.

[triplebig]

Hello Tien,

I switched all the components to basic, and it still gave the same problem. I've tried placing initial conditions, redoing the entire circuit, lowering the time step... nothing works..

here is the LTSpice netlist:

* C:\Schematics\ltspice\Colpitts_osc_2\Colpitts_osc_2.asc
R1 N003 0 3.3k
R2 N001 N003 10k
R3 N001 N002 2.7k
R4 N004 0 1k
C1 N004 0 100n
C2 0 N005 100n
C3 Vout 0 10n
L1 Vout N005 150µ
C4 N003 N005 100n
C5 Vout N002 1µ
Q1 N002 N003 N004 0 2N3904
V1 N001 0 12
.model NPN NPN
.model PNP PNP
.lib C:\PROGRA~2\LTC\LTSPIC~1\lib\cmp\standard.bjt
.tran 0 10m 0 0.01m
.backanno
.end

[Tien_P · Accepted solution]

Hi Triplebig,

I imported the LTspice netlist into Multisim; the only difference is I am using the 2N3904 from the Multisim database instead of LTspice. I've setup the circuit to run Transient analysis.

[triplebig]

That is interesting, so apparently the potentiometer reduces the gain to less than one, not causing the circuit to oscillate...

Can't always trust books it seems.

Thanks!