Stats

  • Locked Locked
  • Replies 11
  • Subscribers 64
  • Views 23757
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

LC parallel circuit at resonant frequency

baristaskin

Dear All,

I am trying to simulate a simple LC parallel circuit when it is drived by a voltage source.

I'm expecting the current of the voltage source V1 to get smaller as its frequency gets closer to the resonant frequency.

When I simulate this circuit at the resonant frequency, with spectre default values, I get:

I tried to play around with the following parameters:

maxstep, reltol, vabstol, iabstol

without success.

My question is: how do I setup Spectre in order to get consistent and accurate results?

What I expect to see is a sine-shaped current signal with no DC value.

I'm including the netlist of the simulation shown above:

// Generated for: spectre
// Generated on: Mar 2 16:11:27 2015
// Design library name: paper3
// Design cell name: LC_osc
// Design view name: schematic
simulator lang=spectre
global 0
parameters _EXPR_8=1.986858915135295e-08 C=1p L=100n vdd=1 \
freqC=503.30696M cycles=10 L_IC=-sqrt(C/L)*vdd/2

// Library name: paper3
// Cell name: LC_osc
// View name: schematic
L1 (Vin 0) inductor l=L r=1a ic=0
V1 (Vin 0) vsource type=sine freq=freqC ampl=vdd/2 sinephase=90 sinedc=0
C1 (Vin 0) capacitor c=C ic=vdd/2
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \
tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 \
digits=5 cols=80 pivrel=1e-3 sensfile="../psf/sens.output" \
checklimitdest=psf
tran tran stop=_EXPR_8 errpreset=conservative write="spectre.ic" \
writefinal="spectre.fc" annotate=status maxiters=5
finalTimeOP info what=oppoint where=rawfile
modelParameter info what=models where=rawfile
element info what=inst where=rawfile
outputParameter info what=output where=rawfile
designParamVals info what=parameters where=rawfile
primitives info what=primitives where=rawfile
subckts info what=subckts where=rawfile
save Vin V1:p L1:1
saveOptions options save=allpub

 

Thank you in advance.

Parents

  • Dear baristaskin,

    Thank you - very helpful information!

    >  This non-linear network has been already used in a cross-coupled LC oscillators as the capacitive load;

    I understand - hence it may be something like a variable capacitive element to modify the frequency.

    > What do you mean by "the voltage source acts as an infinite capacitance"?

    It acts as an energy storage element (i.e., charge source with unlimited amount of charge)

    > 2) I specified that I needed an oscillation of 1V simply to emphasize that I can't use a small signal analysis.

    I understand...

    > What I am trying to do is forcing an oscillation with the voltage amplitude that I decide.

    Are you trying to make the voltage source appear as the source of power to sustain the oscillation?

    > The bottom line is that I am interested in computing the power dissipated by the voltage source, at the resonant frequency of the system.

    I think I'm understanding what you want - you basically want to know how much power is necessary to sustain oscillation at of your non-linear network combined with the inductor.  Effectively, you would like the voltage source to be your "sustaining" amplifier and determine how much power is required. Yes? No?

    The problem with using a voltage source is that it  has zero output impedance. Hence, it will directly impact the natural frequency of oscillation (i.e., its resonant frequency) and you will always be struggling with numerical accuracy issues if you try to force it to the resonant frequency of the network.

    I would approach it by changing the voltage source to a sinusoidal current source. Run a transient simulation at several current source amplitudes over a range of frequencies. The current source has an infinite output impedance and therefore models an ideal "sustaining amplifier". You can determine the power the current source is applying as you approach the resonant frequency. You will need to change the current source amplitude if you are trying to keep a constant voltage swing. It is still a difficult numerical problem.

    With high Q circuits, it is very desirable to consider an analysis where you separate the sustaining amplifier and tank circuits to predict both oscillation and large signal behavior. Negative resistance analyses are designed for this reason.

    I am sorry if my understanding is still not correct - but hope this spurs you with some added thoughts!

    Shawn

Reply

  • Dear baristaskin,

    Thank you - very helpful information!

    >  This non-linear network has been already used in a cross-coupled LC oscillators as the capacitive load;

    I understand - hence it may be something like a variable capacitive element to modify the frequency.

    > What do you mean by "the voltage source acts as an infinite capacitance"?

    It acts as an energy storage element (i.e., charge source with unlimited amount of charge)

    > 2) I specified that I needed an oscillation of 1V simply to emphasize that I can't use a small signal analysis.

    I understand...

    > What I am trying to do is forcing an oscillation with the voltage amplitude that I decide.

    Are you trying to make the voltage source appear as the source of power to sustain the oscillation?

    > The bottom line is that I am interested in computing the power dissipated by the voltage source, at the resonant frequency of the system.

    I think I'm understanding what you want - you basically want to know how much power is necessary to sustain oscillation at of your non-linear network combined with the inductor.  Effectively, you would like the voltage source to be your "sustaining" amplifier and determine how much power is required. Yes? No?

    The problem with using a voltage source is that it  has zero output impedance. Hence, it will directly impact the natural frequency of oscillation (i.e., its resonant frequency) and you will always be struggling with numerical accuracy issues if you try to force it to the resonant frequency of the network.

    I would approach it by changing the voltage source to a sinusoidal current source. Run a transient simulation at several current source amplitudes over a range of frequencies. The current source has an infinite output impedance and therefore models an ideal "sustaining amplifier". You can determine the power the current source is applying as you approach the resonant frequency. You will need to change the current source amplitude if you are trying to keep a constant voltage swing. It is still a difficult numerical problem.

    With high Q circuits, it is very desirable to consider an analysis where you separate the sustaining amplifier and tank circuits to predict both oscillation and large signal behavior. Negative resistance analyses are designed for this reason.

    I am sorry if my understanding is still not correct - but hope this spurs you with some added thoughts!

    Shawn

Children
No Data

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.