Connect with us

HSPICE to PSPICE Conversion

Discussion in 'CAD' started by Gish, Feb 19, 2005.

Scroll to continue with content
  1. Gish

    Gish Guest

    Hi Guys

    I have some SPICE code that runs perfectly in HSPICE but will not run
    in PSPICE due to issues with "subcircuit expansion." If there's any
    experts out there who could take a quick look at this and let me know
    what the issue might be I'd appreciate it.

    Thanks


    ******************************************************
    **** circuit description
    ******************************************************
    rs in inp 50
    r1 inp vss 1K
    x1 inp inm out vss my_opamp
    rf out inm 100K
    r2 inm vss 1K
    ******************************************************
    **** parameters section
    ******************************************************
    ******************************************************
    **** sources section
    ******************************************************
    v1 in vss sin(0V 60mV 10x 100ps 0)
    v2 vss 0 dc 0V
    ******************************************************
    **** specify nominal temperature of circuit in degrees C
    ******************************************************
    ..TEMP= 60
    ******************************************************
    **** analysis section
    ******************************************************
    ..tran 1ns 200ns
    ..END
     
  2. Chaos Master

    Chaos Master Guest

    19 Feb 2005 12:41:24 -0800: Gish (----> ) ---->
    sci.electronics.cad @
    What's the model for 'my_opamp' subcircuit (subckt)?

    []s
    --
    Chaos Master®, posting from Canoas, Rio Grande do Sul, Brazil - 29.55° S
    / 51.11° W / GMT-2h / 15m .

    "People told me I can't dress like a fairy.
    I say, I'm in a rock band and I can do what the hell I want!"
    -- Amy Lee

    (My e-mail address isn't read. Please reply to the group!)
     
  3. Gish

    Gish Guest

    Ok,

    I actually figured everything out except for one line...

    E1 out ref in+ in- MAX=5V MIN=-5V opamp_gain

    I'm trying to code a VCVS with maximum and minimum output values, but
    PSPICE rejects the MAX and MIN parts. Any ideas?

    Thanks
     
  4. Chaos Master

    Chaos Master Guest

    19 Feb 2005 20:25:20 -0800: Gish (----> ) ---->
    sci.electronics.cad @
    I think that PSpice doesn't support MAX and MIN values.

    []s
    --
    Chaos Master®, posting from Canoas, Rio Grande do Sul, Brazil - 29.55° S
    / 51.11° W / GMT-2h / 15m .

    "People told me I can't dress like a fairy.
    I say, I'm in a rock band and I can do what the hell I want!"
    -- Amy Lee

    (My e-mail address isn't read. Please reply to the group!)

    For spammers: , or .
    Those await for your spams!
     
  5. Jim Thompson

    Jim Thompson Guest

    [snip]

    Here are a few of the operators in PSpice BEHAVIORAL elements:

    LIMIT(x,min,max) result is min if x < min, max if x > max, and x
    otherwise

    MAX(x,y) maximum of x and y

    MIN(x,y) minimum of x and y

    In addition you must use the BEHAVIORAL syntax of the E-source

    So the correct expression for E1 is:

    E1 out ref VALUE = {LIMIT((opamp_gain*V(in+,in-)),MIN,MAX)}

    ..PARAM MAX=5V MIN=-5V opamp_gain=100K

    (Or put the numerics directly in the expression.)

    This is convergence risk using mathematical limits, since they are
    hard, and derivatives don't exist at the limit points.

    I prefer using the TANH expression:

    E1 1 0 VALUE {(tanh(A*V(INP,INN))+1)/2}
    E2 OUT 0 VALUE {V(1,0)*(VP-VN)+VN}

    ..PARAM A=100K ; OpAmp Gain
    ..PARAM VP=+5V ; Positive Limit
    ..PARAM VN=-5V ; Negative Limit

    (Note that exact gain is an interaction between A, VP, and VN (E1
    produces 0 ->1), but I'm still too sleepy this morning to make an
    exact expression :)

    ...Jim Thompson
     
  6. Jim Thompson

    Jim Thompson Guest

    [snip]

    Are you using PSpice "raw", i.e. without schematic capture?

    Both PSpice Schematics and Capture (gag me with a spoon) have the
    correct netlist TEMPLATE contained within the symbol.

    (Not that I should be one to criticize. I went for MANY years drawing
    schematics with pencil and paper, numbering nodes, hand-typing
    netlists, and batch-loading into Berkeley Spice 2G6 on an old VAX,
    IIRC, 1170. Then I discovered PC's and bought my first 386 for $6K...
    cheap because it was a clone :)

    ...Jim Thompson
     
  7. Chaos Master

    Chaos Master Guest

    Sun, 20 Feb 2005 10:40:10 -0700: Jim Thompson (---->
    ) ----> sci.electronics.cad @
    I sometimes end up doing this, even though I have 2 schematic editors
    here (LTspice and SIMetrix Intro).


    []s
    --
    Chaos Master®, posting from Canoas, Rio Grande do Sul, Brazil - 29.55° S
    / 51.11° W / GMT-2h / 15m .

    "People told me I can't dress like a fairy.
    I say, I'm in a rock band and I can do what the hell I want!"
    -- Amy Lee

    (My e-mail address isn't read. Please reply to the group!)

    For spammers: , or .
    Those await for your spams!
     
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

-