Hello, I am currently working on a wireless charger prototype for my senior design course. I am currently working on the oscillation portion so I will be able to create an inductive coupling with two coils.

I have this circuit on the pspice but all I am getting is a flat DC output. Anyone have any suggestion to fix this problem? This is very similar to this thread, but that is an older thread. http://forum.allaboutcircuits.com/threads/common-base-colpitts-oscillator.72724/

 

Previous experience tells me that your L to C ratio is way off; you do better to have a much lower L and much higher C to keep the same L*C product, but have a tuned circuit with a much higher Q. I am modelling a lossy inductor with a series resistance of 20mΩ.

Also, your feedback (Xc10/Xc9) is much too high.

So here it is running. Note the distortion, which is typical for a Colpitts.



The start-up behavior is as shown here:

 

Thank you for the help! Its strange, im still getting the same problem of basically a DC output. I will have to continue testing the circuit with different values to see if that helps.

 

Sometimes an oscillator simulation will not start because the initial DC operating point part of the simulation finds a quasi-stable state with no oscillation (which would not likely occur in a real circuit due to intrinsic circuit noise).

Try using the Use Initial Operating Conditions option (.uic) to see if that helps.

Otherwise you can put a voltage source in series with the transistor base to generate a small single pulse (say 1V) at the beginning of the simulation to kick-start the oscillation.

 

Try two things:

First, set the total simulation run time to about 20 of the expected cycles of oscillation; in this case about 30us. When I do that in LTSpice using the .TRAN 2ou directive, this is what happens: (all other things being as they are in post #2)



Alternatively, leave the sim run time long (at 5ms, many, many cycles of oscillation), but force Spice to take little tiny steps (overcome Spice's time-step-control algorithm by specifying the minimum step command thus: .tran 0 5m 0 1u If you accept the default Spice time-step, it gets so big quickly that Spice misses the tiny perturbations that are taking place (math noise), which gets amplifed, which starts the oscillation.

Yet another way of forcing a Spice sim of an oscillator to start is to put an initial condition inside the LC tank circuit. Adding this directive .IC I(L1) = 1f (set an initial current of 1femtoA in the inductor) creates enough of an initial perturbation to get it started.