Connect with us

Measure impedance with spice cad program?

Discussion in 'CAD' started by rob, Sep 12, 2003.

  1. rob

    rob Guest

    Hi to all.
    I was wondering if it is possible to measure impedances directly with
    programs
    like LTspice or Orcad.
    For instance:
    When simulating a class a small sig amp I would like to be
    able to click on the base and have the simulator show the input
    impedance.
    You can measure voltage and current no problem , so I assume there
    should be a way to show impedance.
    Cheers
    Rob
     
  2. I don't think any Spices are that easy. You generally have to do a
    manually set-up of V/I.

    In SuperSpice, you can use the AC sweep set-up to specify a source as an
    impedance source, and it will automatically do a plot of input/output
    impedance at that point without any other setting up. There is an
    example impedance.sss.

    Its a nice idea, I might add it in. SuperSpice does do this already for
    power, that is alt-clicking on the device will plot is power.

    Kevin Aylward

    http://www.anasoft.co.uk
    SuperSpice, a very affordable Mixed-Mode
    Windows Simulator with Schematic Capture,
    Waveform Display, FFT's and Filter Design.
     
  3. Jim Thompson

    Jim Thompson Guest

    For *impedance* force an unit AC current into the node, then display
    Real and Imaginary parts of the resultant voltage.

    For *admittance* force an unit AC voltage onto the node, then display
    Real and Imaginary parts of the resultant current.

    ...Jim Thompson
     
  4. Hi,
    TINA PRO has a facility for directly reading the real or complex
    impedance of a circuit node. Their URL is -

    http://www.tina.com/


    Cheers - Joe
     
  5. Rob,
    It's probably much easier to just write this type of spice device
    without using xspice. That's been my experience anyway. Integration
    of the general non-linear capacitance isn't too hard to figure
    out. LTspice has an arbitrary capacitance device that is useful for
    rapid prototyping new charge models. I'm not much of a fan of xspice
    and I have not seen it used by the major SPICE programs like LTspice,
    PSpice, hspice, or Spectre.
    There's various books on how SPICE works, the 2nd edition of the one
    JT suggests is one I always recommend and you will need, but doesn't
    address SPICE internals. A good one there is the one by Pillage and
    Rohrer. I've been thinking of writing one myself, but until then
    you should just get every one you can find if you want to get involved
    in this. It's a interesting endeavor. You'll find yourself in club
    smaller than the number of people that walked on the moon.

    --Mike
     
  6. The Captain

    The Captain Guest

    In Pspice/Schematics you can set both voltage and current probes at
    the point where you want to measure impedance. For the real part of
    the impedance you simply add a trace once you run the simulation
    labelled V(x)/I(x) which will give you the resistance of the point
    being probed. This is best done in an AC analysis which has the
    advantage of showing you the frequency response of the real portion of
    the impedance as well.

    The next step is to run the same model with a voltage phase probe at
    the measurement point. This is available in Schematics in "Markers",
    "Mark advanced". This, for obvious reasons, only works with an AC
    analysis. You will now have the resistance and phase, at all relevant
    frequencies, from which you can calculate any other parameters.

    This works in Pspice/Schematics. I don't know about other versions of
    Spice, but I would assume something similar is available.

    John
     
  7. rob

    rob Guest


    Thanks for the help guys
    Rob
     
  8. ddwyer

    ddwyer Guest

    I also have an application for measuring the negative real part of the
    input resistance to the terminals of a crystal (or LC) one port
    oscillator.
    I measure the (complex) volt drop across a low value resistor placed
    between a frequency swept signal source and the oscillator terminals; LT
    spice did not like negative resistors but I managed to overcome this by
    shunting with enough resistance to ensure the result was always
    positive.
    Pierce oscillators and similar exhibit a negative resistance maxima
    dependent on the frequency and capacitor values, this provides a good
    means of determining the max crystal esr
    that can be made to oscillate.
     
Ask a Question
Want to reply to this thread or ask your own question?
You'll need to choose a username for the site, which only take a couple of moments (here). After that, you can post your question and our members will help you out.
Electronics Point Logo
Continue to site
Quote of the day

-