Connect with us

SPICE model for PVI1050N

Discussion in 'CAD' started by Christian HOSTELET, Jun 24, 2004.

Scroll to continue with content
  1. Hello,

    I'm desperately looking for a SPICE model of the photovoltaic
    isolator PVI-1050N from International Rectifier. I asked their
    support desk but got a negative answer. Has anyone built such a
    model? Or is it possible to build one using the information given
    in the datasheet?

    Thanks
     
  2. Ken Smith

    Ken Smith Guest

    Making your own model shouldn't be too hard.

    The input side is an LED. I doubt you need to model any AC parameters on
    that side. Just get the drops right.

    The output side is a stack of photo diodes. You get a current equal to
    about 1/1000 of the LEDs current out. There is a large diode leakage
    current and capacitance in parallel with this. You may be able to get
    away with just the output current and leakage. The capacitance of the
    MOS-FET you hook it too is sure to be the controlling effect.
     
  3. (Ken Smith) écrivait
    Ken,

    Thanks for your reply, but I'm still a newbie on Spice.

    OK for the input side (LED) it seemed relatively straightforward.
    Same for the isolation resistance and capacitance.

    I'm less confortable with the photodiodes stack.
    In the datasheet there is a Voutput=f(Iinput, Rload) diagram which is
    rather clear, but I'm having difficulties to translate that to the
    appropriate current source(s) and/or voltage source(s) controlled by
    the load and LED currents.
    Maybe I'm too much looking for perfection.
    Anyway, I want to study the transient aspects in using this component
    with a pair of MOSFET (bi-directional switch) and don't want to
    overlook some important characteristics in the modelling.

    Any help appreciated
     
  4. Ken Smith

    Ken Smith Guest

    Could be you are going for needless perfection.

    I haven't got the data sheet in front of me but I suspect that the easiest
    way to develop the model is to:

    (1)
    Make a current controled current source that will give you the right short
    circuit currents. To do this you put a voltage source (perhaps set to
    zero) in series with the LED to measure the current. You then code it
    like this:

    F1 OutputNode1 OutputNode2 VcurrentSense Gain

    or

    F1 OutputNode1 OutputNode2 VcurrentSense TBL(0 0 in out in out .. etc)

    Where "in" and "out" are the currents on the LED and the output side.


    (2)
    Make a voltage controlled current source to load the output of the current
    source to get the open circuit voltage right. This will be a "G" element.
    You could also try just loading the output with a string of 1N914s. I
    guess about 18 of them.

    (3)
    Plot the results and dream up something to get the difference between what
    the model does and the part does and tack it in. I don't think this will
    even be needed.
     
  5. A resistor is simpler:)
    Ahmmmm...famous last words...

    I have had a little play with this. I had a look at the graphs. They
    show an output graph something like the output characteristis of a
    transister, but Vce being replaced by the input current. This implies
    some sort of limiting. However, into a s/c the current follows the input
    with a scale factor, requiring limiting to be removed.

    What I have done here, is use an iout=i/(i+K) to form a limiter, but
    multiplyed K by the output voltage such that as V goes to zero the
    limiting goes away.

    The graphs are roughly of the right shape with different loads (1M to
    10M to open and under s/c conditions, but I have not tweaked them yet.

    Preliminary idea PVI15080N:
    *************
    ..subckt PVI anode cathode out_plus out_neg
    *
    *copyright kevin aylward, www.anasoft.co.uk.
    *this model can be freely used provide this notice is included
    d1 anode sense1 dmod1
    vsense sense1 cathode 0
    biout out_plus out_neg i = -0.001 * i(vsense)/(1 + 80 * i(vsense) *
    v(out_plus, out_neg))
    rout out_plus out_neg 5Meg
    dout out_neg out_plus dmod2
    ..MODEL dmod1 d(rs=10 cjo=2p is=100p N=2.5 bv=7)
    ..MODEL dmod2 d(rs=10 cjo=2p is=100p N=1 bv=30)
    ..ends PVI
    **********

    I have ignored the output string of diodes for now. I have only spent a
    little while on it, so there may be a better way or more accurate way.
    The "80" and "5Meg" need to be twiddled to get the best match.

    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.
     
  6. "Kevin Aylward" <> écrivait

    [snip]
    Looks great !

    I'll play with it, especially the B function.
    For Rout, it seems to be a linear function (or inverse of) of the input
    current i(Vsense). I'll look at that.
     
  7. Well, I just used a fixed resistor. The basic vout verses Iin shapes are
    ok as the load resister changes. Do a DC sweep of 0 to 20ma, then param
    step the load from 2M to 10 meg. The equation wants a bit more of a
    tweak to get a better fit though.

    The turn off response really needs an additional term. The data sheet
    shows a turn off speed independent of load resister. Not sure why this
    should occur. I havent looked at the physics of these things yet.

    I tweeked the diodes a bit as as well

    ..MODEL dmod1 d(rs=10 cjo=10p tt=1n is=10u N=6 bv=7)

    ..MODEL dmod2 d(rs=10 cjo=10p is=1u N=1 bv=15)

    To get a better match on typical leakage, but this data is guestimated
    as well.

    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.
     
  8. Kevin,

    (NB: My "referential" is IR's datasheet N° PD10054-B)

    I tried with your new diodes models (dmod's), but it seems to be
    incorrect (output voltage divided by 2 ..?). Keeping your former diodes
    models, and adjusting Rout to 5.4Meg and i(vsense) coefficient to 0.0008
    (instead of 0.001), I got very correct results for VDC = f(Input
    Current) (ref. Fig.1 in datasheet)

    I've stepped using 0, 1MEG, 2.2MEG, 4.7MEG, 10MEG and "infinite" Rload
    with Input Current sweeping from 0 to 20mA.

    I've also introduced a temperature coefficient K=1-0.009*(TEMP-27) for
    the Biout current equation to take in acccount this parameter.

    Now there is the time response. Couldn't find the IR's definition of it.
     
  9. Strange. I suspect operator error. It works ok on my set up. Try one at
    a time. dmod1 has its IS to be 1/10 of the data sheet maximum, which
    meant that N had to be increased. These values are guestimated because
    typical are not specified.
    I picked the other model because the numbers were rounder.
    There is a graph. It shows various torn times, with essentially a
    horizontal line for turn off.

    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.
     
  10. Sorry, should have been clearer (I'm not native).

    I've seen the graph but what I'm missing is the definition of Ton and
    Toff. Is it 3dB, 10-90%, something else?

    Anyway, I'll try again with the modified Dmod.
     
  11. Its the 10%-90% points.


    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.
     
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

-