need help self excited class c oscillator simulation and lts

[nanotech1]

i have a problem i need to do a simulation of a self excited class c
oscillator with ltspice

when i run the circuit in ltspice it doesnt oscillate
in simulation run mode does ltspice needs a special directive to work with
this type of oscillator

in the ltspice demo folder they are some other oscillator circuit example
( colpitts , hartley ) and these do work fine
in simulation mode run but there isnt any example circuit for armstrong or
blocking osc in the demo folder

i just want to know how to setup ltspice for any of the above osc circuit
any help appreciated

 

[Jonathan Westhues]

"nanotech1" <nortronics@sympatico.ca> wrote in message
news:4_jbe.1577$BW6.515997@news20.bellglobal.com...

i have a problem i need to do a simulation of a self excited class c
oscillator with ltspice

when i run the circuit in ltspice it doesnt oscillate
in simulation run mode does ltspice needs a special directive to work with
this type of oscillator

A system with positive feedback and a loop gain greater than 1 at a
particular frequency will sustain an oscillation at that frequency, so that
once it is oscillating it will continue to oscillate. Something has to start
the oscillation though. In a real circuit there will always be some noise to
get it going, but in SPICE that is not necessarily the case.

You could try telling SPICE to solve for the initial operating point with
the independent sources off, and then to turn the sources on at the
beginning of the simulation. Whatever transient that causes will hopefully
be enough to start the oscillation. You can do that with the "startup"
directive (which I see that they used in some of the examples).

Other options include: replace all your DC sources with PULSE(...) sources
that are off for the first few microseconds and then turn on and stay on;
specify an initial condition on a capacitor or inductor in the loop; specify
a smaller max timestep, one much smaller than your expected period of
oscillation.

Jonathan
http://cq.cx/

 

[Bob Eldred]

"nanotech1" <nortronics@sympatico.ca> wrote in message
news:4_jbe.1577$BW6.515997@news20.bellglobal.com...

i have a problem i need to do a simulation of a self excited class c
oscillator with ltspice

when i run the circuit in ltspice it doesnt oscillate
in simulation run mode does ltspice needs a special directive to work with
this type of oscillator

in the ltspice demo folder they are some other oscillator circuit example
( colpitts , hartley ) and these do work fine
in simulation mode run but there isnt any example circuit for armstrong or
blocking osc in the demo folder

i just want to know how to setup ltspice for any of the above osc circuit
any help appreciated

It seems to me that class C is problematic because the natural quiescent
state is off, no current flow. Unless there is a large turn on transient or
noise spike, the circuit will never transisition through its active region
where gain occurs. Therefore regeneration and oscillation may never start. I
think spice sees that, the initial state is off and it stays off. There is
nothing to "push" the circuit into its active region. Aren't most
oscillators of the types you mentioned class A or maybe class B where their
initial state is somewhere in the active region of amplification? Maybe you
should design your circuit where it starts class A then transitions to Class
C as oscillation builds up. This can be done by using the oscillation,
rectified to produce the class C bias required.
Bob