Tuned Amplifier in LTSpice

Hi everybody.

I'm trying to simulate a tuned amplifier in LTSpice in order to get a better grasp on its operation.
This is a first step in my studying of oscillators.
Anyway, I am getting weird results that I am not able to explain.
I would be very grateful if some of you guys could help

I'd love to attach my .asc file but apparently, I can't. But here is a picture of the setup:


I'm am using the MOS model from cmosedu.com available here, in particular the N_1u model.

There are actually several things I don't understand in the results I get from those simulations.
For now, I am gonna focus on the one that most annoys me: the result of the transient simulation for V(out)
depends (a lot) on the max timestep (dTmax: 4th parameter of the .TRAN command line) as shown below

With a max timestep of 1ns, i get:


Here, in the permanent regime, the peak-to-peak amplitude of V(out) is 11.95mV which
is approximately what I expected. In my understanding, at the resonnace, the gain of the tuned amp
should be slightly higher than the one of the common source (wich is 11.76mV) since DC level of Vds is higher.

Now, with a max timestep of 50ns (still 40 times lower than the signal period), I get:


Not only the transient part of the response is quite diferent,
the amplitude in the permanent regime is now 1.2mV!
Here is a zoom of the permanent regime (same plot as above, only zoomed)


Does anyone have any ideas about why this is happening? I am a bit confused.

Thanks all in advance.

Pif

Where is the biasing of the MOS ?? What about the Load ??
What is your intention exactly ??

BigBoss said:

Where is the biasing of the MOS ??

Click to expand...

The input voltage has a 1V offset which, as DC simulation told me, is an acceptable bias

BigBoss said:

What about the Load ??

Click to expand...

what about it?

BigBoss said:

What is your intention exactly ??

Click to expand...

That's a good question whose answer is not that obvious
I just want to see if simulation gives me the result I expect.
In particular, that at the resonnant frequency, the gain of the tumed amplifier is
approx. the same as the gain of the common source.

The suggested method to attach .asc files and other file types unknown to the Edaboard file manager is to zip it.

Why does max timestep affect the simulation waveform? You know that your circuit has huge Q near to 1000, you have adjusted the stimulation frequency precisely to match the resonance. One explanation is that timestep changes the effective resonance frequency by a small amount, thus detuning the circuit. Factor 40 is apparently not enough to simulate the circuit behaviour precisely.

Consider that a regular LC oscillator won't achieve this high Q, why not using a more realistic figure?

Thank you very much!!

Next time I'll attach a zip.. thx.

I don't understand the mechanics behind the transient simulation enough to understand how its timestep
can modify the resonance frequency. I need to study a bit

Don't you think that this is the effective frequency of the signal that could be changed a bit?

If the bias is correct why 5V appears at D-S even a resistor is used as a load ?? There should be voltage drop over 200 Ohm resistance.
But mean value is still 5V that is equal to VDD.. There are somethings go wrong..
Mean value had to be Vds=Vdd-Idsq*Rd right ?? This is for CS configuration.Check the second one under this circumstance.

Well, actually, it seems to me that the inductor keeps drain's DC level at 5v.
This is why, as I mention in my first post, I expect a slightly higher gain in the tuned amp.
compared to the gain of the CS.

- - - Updated - - -

FvM said:

Consider that a regular LC oscillator won't achieve this high Q, why not using a more realistic figure?

Click to expand...

Yes, I'm gonna reduce the Q. I wasn't really focusing on it until now..
I just wanted to confirm the behaviour at the resonance frequency.

Other strange thing is that while DC and transient simulation give the same gain,
for some reason, AC simulation shows a slightly inferior gain value.

I finally attached the .asc file.

Thanks again to both of you

View attachment tuned_amp.asc.zip

Well, actually, that was the window size that was messing around.
with .option plotwinsize=0, it works like a charm...

Why are you adjusting the transient max timestep value?
Normally that value is left blank and Spice adjusts that to the proper value, depending upon the rate of voltage change versus time in the simulation.

crutschow said:

Why are you adjusting the transient max timestep value?
Normally that value is left blank and Spice adjusts that to the proper value, depending upon the rate of voltage change versus time in the simulation.

Click to expand...

Cause if I don't, the results are nonsense. like this:


the pk2pk amplitude here is 170uV...



Actually, it still doesn't work properly even with plotwinsize=0.
The same problem seems to occur even when simulating
the tank with a current source only.

Don't understand why it's happening, but it surely is a known phenomenum.
Gonna seek more about that.

I've seen very similar issues when doing transient simulations of high-Q circuits in LTspice (though it's likely not an issue particular to LTspice, but numeric solvers in general).

Basically, whatever timestep you would normally expect to need for the resonant frequency (like maybe 500ns for you 500kHz resonant frequency), divide that by Q to ensure decently accurate results.

Or, like FvM suggested, give your circuit a more realistic Q factor.