CMRR, PSRR Simulation

Discussion in 'Cadence' started by Gundam, Sep 17, 2008.

  1. Gundam

    Gundam Guest

    Hi all, just quick question here. I am using the simulator Spectre. I
    am wondering if there is any direct setting or build in function to
    simulate CMRR and PSRR for an amplifier design. The way I did is to
    set up common mode and differential mode signal source to simulate and
    have their gain ratio. Similar way is for PSRR. Is there any other
    faster or more automatic method in Cadence? The other quick question
    is to simulate input referred noise. I plot the input noise
    distribution throughout the whole frequency band, and I just integrate
    over the frequencies of interest to get a number. Does it make sense
    or there is another better way in Spectre simulator? Thanks for all
    Gundam, Sep 17, 2008
  2. Gundam

    Riad KACED Guest

    Hi Gundam,

    I'm not aware of any calculator/ocean built-in function that does the
    measure of the rejection ratios as you are looking for.
    The automated way I could see to make this is to write an ocean script
    and measure the gain of your output at the desired frequency.
    Let's see what others would go for ...

    Riad KACED, Sep 17, 2008
  3. Riad KACED wrote, on 09/17/08 23:05:
    I would strongly recommend using "xf" analysis to do this rather than "ac"
    analysis. With xf analysis you specify the output nodes (or current probe) and
    it will allow you to access the gain from each source in the circuit - so in the
    same simulation you can see the gain from the power supplies and from the input
    signal. There's no need to set an "ac magnitude" on any source.

    If you do it via "ac" analysis, you have to keep changing the source which has
    got ac magnitude (often set to "1") in order to find the gain from that point to
    the output.

    Then computing the rejection ratios should be a relatively straightforward


    Andrew Beckett, Sep 18, 2008
  4. Gundam

    marcoballins Guest

    Can you adapt somhow "xf" analysis to compute rejection ratios in a
    fully-differential architecture?
    I am right now using "ac" analysis because I have to compute among

    ; CM input
    vsc = (VF("/vs+") + VF("/vs-"))/2

    ; CM and DM outputs
    vod = VF("/vo+") - VF("/vo-")
    voc = (VF("/vo+") + VF("/vo-"))/2

    ; Common-mode gain
    Acm = voc/vsc

    ; Common-mode-to-differential-mode gain
    Acmdm = vod/vsc

    Kind regards,
    marcoballins, Sep 24, 2008
  5. Hi Marco,

    This could be done - but you'd need to have single signal sources that you could
    use to represent vsc - a matter of how you organize your testbench. Also, you'd
    probably need a vcvs to get the "voc" equivalent (vod is no problem, because the
    xf output is a pair of nets).

    In other words, providing you have a source to set the common mode level, and
    maybe a source for the differential input, it should be doable. But you might
    find it easier to do with AC in this case, although you then have to keep moving
    your "AC" source between runs.

    Normally the problematic case for xf/pxf type analyses is when you have
    quadrature inputs, rather than differential, as you can't really reformulate
    them into single signal sources.


    Andrew Beckett, Sep 29, 2008
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.