Common Source AC Sweep

Discussion in 'General Electronics Chat' started by newbie217, Nov 27, 2010.

  1. newbie217

    Thread Starter Active Member

    Apr 12, 2009
    52
    0
    Hi,

    I'm trying to simulate a Common Source example from Sedra and Smith, 5th edition, page 293.

    The model parameters used are: vto = 1.5, kp = 0.25m, lambda = 0.02

    I notice that when I do the DC bias simulation, the numbers I get are matching hand calculations. That is:

    ID = 1.06 mA
    VDS = 4.4 V = VGS
    ro = 47k
    Av= -3.3

    If I do an AC sweep w/ the input signal = 1 VAC amplitude, then I get Av = -3.50 or so (close to hand calculations). However, if I increase the amplitude to say 10 V or 100 V, then the output voltage is coming out to be over 346 V. This doesn't make much sense, obviously. Plus the transistor would have been out of the active region long ago when: vds < vgs - vt.

    I'm just trying to figure out what results the simulation is giving me. I would think that the output voltage would plateau while operating in the triode region, not keep rising as the simulation is showing me. What am I doing wrong?

    Thanks!
     
  2. Jony130

    AAC Fanatic!

    Feb 17, 2009
    3,962
    1,097
    Becaues in PSpice AC sweep is small-signal analysis.
    And in the small-signal you have linear amplifier with gain -3.50V/V.
    If you want to check max output swing you must use transient analysis.
     
  3. newbie217

    Thread Starter Active Member

    Apr 12, 2009
    52
    0
    Could someone please provide an example on how to do an effective transient analysis to observe maximum input signal / maximum output swing? What kind of input source should you use? For example, a sinewave w/ 1.0 V amplitude? I would really appreciate it :)

    So, for a 1 VAC input source, the gain is 3.5. But this doesn't tell me whether the transistor is in the active region or not? That doesn't seem very useful. How would I relate the transient time-domain analysis w/ the frequency analysis? Say for example, the maximum input signal that can be applied is 300 mV. Where does this information show up on the AC analysis? How do I relate the two?
     
  4. thatoneguy

    AAC Fanatic!

    Feb 19, 2009
    6,357
    718
    What software are you using?
     
  5. Jony130

    AAC Fanatic!

    Feb 17, 2009
    3,962
    1,097
    I repeat AC sweep is frequencydomain analysis using ideal small-signal model.

    If you must do time-domain analysis to get max output voltage.
    For example I use Schematics and transient analysis of your amplifier.
    For Vin = 10Vp and 0.3Vp
     
    • 11.PNG
      11.PNG
      File size:
      22.7 KB
      Views:
      29
    • 12.PNG
      12.PNG
      File size:
      20.6 KB
      Views:
      27
    • 10.PNG
      10.PNG
      File size:
      54 KB
      Views:
      29
    Last edited: Nov 27, 2010
  6. newbie217

    Thread Starter Active Member

    Apr 12, 2009
    52
    0
    thanks jony for your help.

    I still don't feel like I have a real good grasp of the overall concept though. By using the transient analysis, I can see that at 10 V the output is severely distorted compared to the input. But I am still looking for a more mathematical expression / relationship to the AC analysis. Otherwise I will be going about this the wrong way doing simple trial and error techniques.

    I copied the data from the waveform and pasted it to Excel. I found that for the 0.3 V amplitude case, Vout/Vin ~ 3.5 (expected by hand calculations).

    For 10 V amplitude, Vout/Vin there is a lot of variation and Vout/Vin is less than 1 for the most part.

    However, the AC sweep for 10 V is showing me a gain of 34 for 1 khz sinewave, amplitude 10 V. This is the source of my confusion. How can I relate the two findings mathematically?
     
  7. newbie217

    Thread Starter Active Member

    Apr 12, 2009
    52
    0
    Here is the data I took from the waveform viewer.

    Btw, using OrCad Capture Lite version 9.2. thanks.
     
  8. Ron H

    AAC Fanatic!

    Apr 14, 2005
    7,050
    657
    In Spice, AC analysis first calculates the quiescent state (DC voltages and currents) of a circuit, and then creates a linear model of gain, impedances, etc., at that quiescent state. You can then apply any AC voltage to the input, and the output will appear multiplied by the gain. If the gain is 10, and you apply 1 microvolt, you will get 10 microvolts out. If you apply 1 megavolt, you will get 10 megavolts out.
    Obviously, this is useless for determining limiting, distortion, etc. It is useful for creating Bode plots (frequency response graphs), and other frequency-dependent parameters of a circuit. You have to know enough about the circuit to realize what a reasonable amplitude range is for real-world applications, which transient analysis will help you determine.
    Since the circuit responds to AC analysis identically at any amplitude, it makes little or no sense, when plotting gain in decibels, to use any input amplitude other than 1V.
     
    newbie217 likes this.
Loading...