Pierce Oscillator simulation in Hspice ?

[Electric_Shock]

I would like to simulate the Pierce oscillator in Hspice but I don't know how to generate a white noise in hspice environment. I also try .ic command to initialize for the circuit but it does not work. How I deal with this simulation ?

 

[LvW]

Why do you need a white noise source?
Perhaps you have learned that noise would be necessary to start simulation?
That`s completely wrong (nonsense)!
To start simulation, you can give one of the capacitots an initial charge (initial condition with some millivolts) or you can inject a short voltage impuls into one of the capacitors (instead of connecting it to ground) .

 

[BradtheRad]

I have experimented with a hardware version of this circuit.
On powerup the first capacitor is positioned so it pulls the input low. Oscillations should start naturally. However all values need to be adjusted, so that the circuit runs as it ought to.

Rf should be high ohms, between 0.5M and 5M. Its behavior combines with the crystal's slight delay. The combined result from their feedback, is to vary the input voltage a little above and below supply/2. The output state snaps up and down.

 

[FvM]

The reason why an oscillator usually doesn't oscillate in a SPICE simulation is that the simulator performs an initial transient solution that puts all nodes in perfect equilibrium. It needs an initial pertubation to get out of equilibrium.

Most simple way is to specify SPICE option uic (skip initial transient solution).

 

[abu_bua]

Perhaps you have learned that noise would be necessary to start simulation?
That`s completely wrong (nonsense)!

I don't think that this is completely wrong. In the crystal you have due to temperature an amount of phonon energy, which acts like noise. Do you have a reference for you statement? In my opinion this noise also makes a contribution during start-up, also it is small compared to the inverter.
During power-up the inverter will be never exactly in equilibrium, because of different parasitic caps, mismatch (K, w/L, ...) and will kickoff the crystal.

However, for simulation to add a noise source (mos noise, resistor, crystal noise) is nonsense, except you want to look for phase noise and jitter issues. For a faster startup it is proper to set initial condition.

 

[LvW]

I did not state that there wouldn´t be any noise.
However, it does not play any role for oscillation start-up.
Each power-on action will produce a transient which is - by far - sufficient to start oscillations.
This is true for simulation as well as hardware reality.
But in case of simulationwe have some additional options (initial conditions, start impuls at a grounded node)

 

[dick_freebird]

Are you sure that HSPICE does not have a voltage source
noise option? Certainly if tnoise analysis is supported there
ought to be a "live" transient noise source.

Failing this, try making a chaotic noise subcircuit with some
combination of paralleled noise+resistor sources that give
you a roughly-right spectrum. You probably don't need a
true white noise source, rather a rack that hits a few
points per decade.

 

[FvM]

The original question of this thread is how to manage oscillator start-up in SPICE simulation. Adding a transient noise source isn't the usual solution. A different question is if it could work under circumstances.

A real electronic oscillator does in contrast to a simulation model not suffer from limited numerical resolution. Thus a linear circuit that fulfils the oscillation condition can start out of perfect equilibrum with the help of circuit noise. As already mentioned, this is a purely theoretical consideration. In practice there will be always a deviation from equilibrium and the noise isn't needed.

I believe I first heard about "oscillator start-up by noise" in university lessons.

 

[BradtheRad]

I often see a similar problem in Falstad's simulator, when I have one or more invert-gates in an oscillator. I find it helps regular oscillations to begin, if I give the input a brief connection, through a high-ohm resistor, to the +V supply. If that does not solve it then I try 0V ground briefly. If that does not solve it then I try applying various volt levels from a potentiometer between +V and ground.