Connect with us

Two questions about LTSpice

Discussion in 'Electronic Design' started by Marco Trapanese, Oct 17, 2012.

  1. Guys, I know most of you are experienced users of spice here :)
    Two short questions, I've already RTM without find the answers.

    - I need a TIP 122 model... where I should look for?

    - worst-case scenario: I set the tolerances of my resistors. How to run
    a simulation to get the worst-case? I'm talking about the maximum span
    of selected traces when components reach their end values.

    Thanks!
    Marco
     
  2. Vlad

    Vlad Guest

    Hello

    For the TIP122, I did a search on Google and I got it within the first hit. As for the worst-case setup, try this link, it has a good explanation: k6jca.blogspot.com/2012/07/monte-carlo-and-worst-case-circuit.html

    Good luck,
    Vlad
     
  3. Il 17/10/2012 08:46, Vlad ha scritto:

    I also got it at the first hit, if you're referring to this page:

    http://www.onsemi.com/pub_link/Collateral/TIP122.SP2

    but the code inside is quite different than the *.asy files available
    into the lib folder of LTSpice. Here my question.

    In fact I've already tried to put the file there calling it tip122.asy.
    But when I select it from LTSpice I got 'Unknown symbol syntax: ".SUBCKT
    Xtip122 1 2 3" '


    Thanks a lot for the link. I'll give it a try.

    Marco
     
  4. o pere o

    o pere o Guest

    The link Vlad provided is a Spice subcircuit file. Perhaps this
    http://www.simonbramble.co.uk/lt_spice/ltspice_lt_spice_tutorial_4.htm
    may help you inserting it into LTSpice.

    Pere
     
  5. Robert Macy

    Robert Macy Guest

    Are you certain you want ALL the worst case values at the SAME time?
    The statistical likelihood of that is supposed to be extremely small.

    We only used the 'worst case box' for milspec designs, where if the
    circuit didn't perform to spec, you had to point tothe component that
    was out of spec, else...

    More likely scenario was for cmmecial designs where we used a Guassian
    distribution for the component tolerances, like 'square root of the
    sum of the squares' tolerances which was quite a bit more lenient to
    design. But even in Production that wasn't realistic - sometimes. We
    found the resistor manufacturers made runs of resistors measured what
    thy made, which created a flat distribution, but then they culled out
    special values which put 'holes' in that distribution! Usually we got
    distributions with the centers cut out. In other words likely to get +
    values and like to get - values, and rarely got exactly what the label
    said.
     
  6. Il 17/10/2012 16:04, Robert Macy ha scritto:

    Small is not zero, and Murphy's watching me :)


    I'm agree, but sometimes is useful to know where are the bounding
    limits, hoping you'll never reach them.

    Marco
     
  7. Il 17/10/2012 08:46, Vlad ha scritto:

    It does the dirty job but in a weird way. I'm going to improve it.
    Do you know a way to obtain the tolerance value already put in the
    related field (e.g. a resistor) ?

    Marco
     
  8. John S

    John S Guest

    There is an example simulation that comes with LTSpice called
    MonteCarlo.asc in the \LTC\LTspiceIV\examples\Educational folder.

    You don't have to do the Monte Carlo, but the example is good to study
    to see how to change component values as you wish.

    Cheers,
    JohnS
     
  9. Hello Jim,

    You can specify a full path.

    Example:

    ..lib C:\mylib1\mosfet\abc.lib

    Best regards,
    Helmut
     
  10. Hello Jim,

    A SPICE-directive is simply a SPICE-line.
    You can either use a SPICE-directive in the schematic or you specify the
    full path in the symbol.

    I personally never use a full path name, because I mostly work on chematics
    for other users. It's then much more convenient to have all files the folder
    of the schemtaic.

    Best regards,
    Helmut
     
  11. Robert Macy

    Robert Macy Guest

    Then there are the 'just get by' values. Where you have them in stock,
    they're almost the right value, but not quite, but it's 12 weeks to
    get the right ones, so you NEED to use these.

    Once when designing an IC, after being told to expect beta of 3:1 and
    not trusting; I designed the circuit to take a beta range of 5:1
    Brother! did THAT pay off!

    Once when designing CCD cameras, and being told to expect a
    'sensitivity' of such and such and again not trusting; I designed to
    accept 50% of the minimum sensitivity. Boy, did THAT pay off.
    Especially when you get a lot in that doesn't meet spec, and there are
    NO others and you're supposed to be shipping 2,000 units/mo and you
    have a room full of workers who will have NOTHING to do if you reject
    that lot.


    So question goes back to the OP...why do you need to design to milspec
    style? Unless your customer is milspec, you have overdesigned for
    instrumentation volumes and probably underdesigned for consumer
    volumes [10,000,000 per year]
     
  12. Charlie E.

    Charlie E. Guest

    Not sure in LTSpice, but in PSpice the worst case sim does this.
    First, it does a base run, and gets your 'output' value. Then, it
    goes to each toleranced part, changes the value a small bit, and runs
    a new sim. It notes whether that output value changes plus, or minus.
    After testing the sensitivity on all the parts, it takes each part,
    adjusts its value in the direction indicated by the sensitivity to its
    limit, and runs a final, worst case simulation.

    Note that this is not necessarily the absolute worst case. In some
    circuits, especially filters, the actual worst case may be a some
    point within the tolerances where resonance effects are worse. Also,
    if you were not careful in setting your distribution types and values,
    you can get wild values for the sim, especially if you have gaussian
    distibution parts (PSpice sets the tolerance as the one sigma point,
    so worst case is three sigmas...)

    Usual practice is to do the worst case high, worst case low, and then
    some Monte Carlo runs. Display them all in the same probe window, and
    you can see what the distribution of results tends to be.
     
  13. Il 17/10/2012 23:57, Charlie E. ha scritto:

    This is the behavior I was expecting. I'm afraid the DIY solution seen
    in the link is not so accurate.


    You're right.


    Ok, I got it.
    Thanks
    Marco
     
  14. Il 17/10/2012 21:13, Robert Macy ha scritto:

    No milspec at all.
    For example, if you followed the thread about the current limiter, I
    want know how much will change the limited current in function of the
    tolerance of the resistor. It's a protection, so I do need to know if it
    will safe with any value I may expect.

    It's just an example, but I hope you understand what I'm saying.

    Marco
     
  15. Robert Macy

    Robert Macy Guest

    Yes, being conservative is good. I used the term 'milspec' merely as a
    descriptor to make it easy to refer to using the worst case box of
    tolerance values. Don't forget to add the tolerances of all the
    measuring intrumentation, too.
     
  16. josephkk

    josephkk Guest

    Poxy hell. I might buy that off you if i could. For obvious reasons it
    is not (reasonably) available for sale by you.


    BTW is PSpice still available for sale? Is the price not too
    unreasonable?

    ?-)
     
  17. josephkk

    josephkk Guest

    You might look at sensitivity analysis. A .sens card with all the
    components you want analyzed listed. Then you could easily pick the ones
    you need to sweep. Myself, i can do most of that in my head without any
    "heavy lifting" analytically.

    ?-)
     
  18. Fred Abse

    Fred Abse Guest

    The file referred is a *subcircuit* file.

    ..asy files are *symbols*, ie. the shape that shows on a schematic.

    Put TIP122.sp2 in /lib/sub, and add the LTspice directive ".lib
    TIP122.sp2" to your LTspice schematic.

    Use the standard NPN symbol, but don't assign a device model. Instead,
    control-right-click on it, which will open a dialog box where you can make
    it into an "X" subcircuit device, and set the appropriate parameters.

    A good read of the manual will make things clear.

    If you use a lot of subcircuit devices, it's a good idea to make a
    dedicated "subcircuit npn" symbol.
     
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

-