Orcad pspice oscillator problem

[kleinesmurf69]

convergence problem orcad

Hello,

I am trying to simulate an oscillator (4MHz) circuit that consists of a transistor and some discrete components. The only thing that comes out of the simulation is in the order of femto to pico volts. Does anyone know what I am doing wrong?

Thanks.

Regards.

 

[flatulent]

convergence problem

This is the result of convergence problems. You should look at the documentation for the program to find the .options statements to use to tighten up the tolerance at each calculated point. reltol and abstol are some of these. Tighten them up by 10x and then 100x if necessary to get the waveform you expect.

 

[boondoggle]

Hi,

You might want to take a look at this document:

http://www.sss-mag.com/pdf/rfosc.pdf

It contains a number of ways to "thump" an oscillator to life in
a SPICE simulation.

-Boondoggle

 

[godz]

Hi,
In such cases, I used to put an Initial Condition (IC) on the oscillator tank, when transient simulation starts the IC represents a disturbance in the oscillator that can trigger the oscillation, but you should take care not to set the IC value too far from the expected DC value of the node otherwise the transient simulation will take a lot of time to reach to the proper DC bias of the circuit.
I also advise you to insert an AC current source at the +ve feedback point of the oscillator and do an AC simulation before transient and notice the output at the tank, if there is peaking in the frequency of interest then the oscillator will probably oscillate when you do transient simulation.
regards,

 

[bastos4321]

Use the inicials conditions in one or two of the capacitors of the feedback network.

Cx n1 n2 xxx IC=1V

.tran 1n xx UIC

Bastos