Connect with us

Why is there no dual gate fets in LTspice?

Discussion in 'Electronic Design' started by LM, Oct 20, 2012.

Scroll to continue with content
  1. LM

    LM Guest

    There are many kinds of them for instance from NXP.
  2. The program must be worth the money. Most software is never effortless no
    matter how much you master it.
  3. LM

    LM Guest

    True. It cant be totally impossible because there are models at NXP. I
    quess I have to start with Yahoo.

    About old simulators. I had in an old 286 machine some similation
    program, Microsim perhaps. It ran about as fast as this windows
    version. LT spice should be about a thousand times faster that it.

    What can do I do with a BF998.prm? (other than perhaps delete)
  4. It does seem vague, just a few lines of Help on the subject. But it's
    straight forward with a little practice.

  5. Hello Jim,

    Open the symbol editor.
    Place 4 pins.
    Right-click on each pin to edit the netlist order to the order in the
    Draw some nice graphic around it.
    Write BFXXX into attribute "Value". Edit -> attributes

    Place this symbol in the schematic.
    Change BFXXX to BF998
    Include the model file with a SPICE-directive
    ..lib name_of_file

    Wire the complete circuit.
    RUN the simulation.

    I have used BFXXX in the symbol, because I had in mind to use it for BF996,
    BF999, BF???.
    If I had used BF998 in the symbol editor, I wouldn't have to change it
    later in the schematic of course.
    It's also possible to make a symbol only for the BF998.
    Last but not least you can already specify the model file in the symbol too.

    Best regards,
  6. Robert Macy

    Robert Macy Guest

    MicroSim was so good I even sprang for the $100+ manual to go with the
    'student' version.

    As you may know, paying for ANY software rankles me to no end. But
    PSpice was so good, I both rewarded MicroSim by buying the book and
    enabled me to create models.
  7. Robert Macy

    Robert Macy Guest

    I still have AND USE my DOS version. Why? because it has the ability
    to plot BH Curves directly

    * model uses MKS and CGS units of cm and cm^2 for input
    * plot converts to Gauss and Oersteds for output
    * to plot, set Y = B(K1) and X = H(K1)
    ..TRAN 1 6 0 1000uS
    ..OPTIONS ITL5=0
    I1 0 1 SIN(0 .1 1 1)
    I2 0 1 SIN(0 .2 1 2)
    I3 0 1 SIN(0 .8 1 3)
    R1 1 0 1
    L1 1 0 200
    K1 L1 .9999 KBREAK
    ..model KBREAK CORE(AREA=3.27156 PATH=12.90399 GAP=0
    +K=100 MS=97772.47 A=500 C=0.2)

    wish LTspice did something like that.

    drew it on paper?! memory slipping? just left to right like playing
    chess in your mind.
  8. Jamie

    Jamie Guest

    You can't do the hysteric core model based on a model first proposed in
    by John Chan ? It's supported in Ltspice. The problem is that mechanical
    data has to be supplied.

    I've been playing with that the last couple of days working with a
    regenerative oscillator, only because I can't figure out how to set the
    turn ratio on the coupled inductors which kinds of screws up my tank
    circuit for a real world example.

  9. LM

    LM Guest

    There are many kinds of them for instance from NXP.
    Most are gone.
    NXP has some low noise dg fets. They are probably easier to use at UHF/
    VHF than a hot 10+GHz XXXfet.
  10. Robert Macy

    Robert Macy Guest

    Apologies to OP, seemed to have hijacked your thread, but please bear
    with us here...

    You missed the syntax of K1 and the ease of plotting BH Curve.

    Although I laud LTspice for using MKS units it can get confusing,
    going back and forth...

    Hc = 1.251 Oe = 99.55 A/m
    Bs = 1.202e3 G = .1202 T
    Br = 85.14 G = .008514 T
    Area = 3.27156 = 327.156e-6 sq m
    Path = 12.90399 = .129039 m
    Gap = 0 = 0 ??

    B from Gauss to Tesla divide by 1e4
    H from Oersted to Amp/m multiply by 79.57747

    then in LTspice you must plot the following 'formulas' to get the BH
    H=NI/pathlength = 1550*I/1A
    Bup = (.1202*(1550*I(L1)+99.55)/(abs(1550*I(L1)+99.55)+99.55*13.12) +
    Bdn = (.1202*(1550*I(L1)-99.55)/(abs(1550*I(L1)-99.55)+99.55*13.12) +
    ,or both, but doesn't work so well
    Bmag = (.1202*(1550*I(L1)+99.55)/(abs(1550*I(L1)+99.55)+99.55*13.12) +
    1.94779e-3*I(L1) + .1202*(1550*I(L1)-99.55)/
    (abs(1550*I(L1)-99.55)+99.55*13.12) + 1.94779e-3*I(L1))/2A

    Can't remember if those are ceneric constants, or constants just for
    THIS model. I either get the 'going up' side or the 'going down side'
    but nothing like I used to get with PSpice DOS version.

    By the way, you'll find that LTspice's curve fit for the Chan model is
    excellent! PSpice's Jiles-Atherton model used to make hour glass
    shaped hysteresis curves that were incredibly difficult to make
    square. But, LTspice does fairly well, by just supplying two terms
    Bsat and the Br [where it hits the axis] and you get a decent looking
  11. Robert Macy

    Robert Macy Guest

    Jim, THAT's uncharacteristically vague.See the reply to Jamie for the
    way to make LTspice do similar plot to what PSpice DOS version used to
    do. I say 'similar' because I have not been able to get the ends of
    the curve to touch each other, get close, but no cigars..
  12. Robert Macy

    Robert Macy Guest

    FOUND IT! this runs on LTspice

    * Plot results as V(12)/1V or V(22)/1V or V(32)/1V vs V(20)/1V
    ..TRAN 1 6 0 10uS
    ..OPTIONS ITL5=0
    * constant absolute permeability = 4pi*1e-7
    ..param uo=1.256637e-6
    * 3C8 material parameters in MKS units
    * Note derived from inspection of Microsim PSpice results
    ..param Hc1=167.1127
    ..param Bs1=.49
    ..param Br1=.4575
    * Specific core parameters in MKS units
    ..param Lm1=.1290396
    ..param A1=327.1756e-6
    ..param Lg1=0
    ..param N1=20
    I1 0 1 SIN(0 .1 1 1)
    I2 0 1 SIN(0 .2 1 2)
    I3 0 1 SIN(0 .8 1 3)
    I4 0 1 SIN(0 1.6 1 4)
    R1 1 0 1
    L1 1 0 Hc={Hc1} Bs={Bs1} Br={Br1} A=327.1756e-6 Lm={Lm1}
    Lg={Lg1} N={N1}
    * From LTspice manual on page 130 and 131 Use B sources to plot
    Bup 12 0 V={(Bs1*(N1*I(L1)/Lm1+Hc1)/(abs(N1*I(L1)/Lm1+Hc1)+Hc1*(Bs1/
    Br1-1)) + uo*N1*I(L1)/Lm1)/1A}
    Bdn 22 0 V={(Bs1*(N1*I(L1)/Lm1-Hc1)/(abs(N1*I(L1)/Lm1-Hc1)+Hc1*(Bs1/
    Br1-1)) + uo*N1*I(L1)/Lm1)/1A}
    Bmag 32 0 V={(V(12)+V(22))/2}
    * assuming flux is contained in the core, H = N1*I(L1)/Lm1
    B_H 20 0 V={N1*I(L1)/Lm1/1A}

    then, plot V(12) and V(22) vs V(20) and you get the hysteresis curve,
    but the ends don't connect.

  13. Robert Macy

    Robert Macy Guest

    found it! see the reply to myself to Jamie.
  14. You can define the subckt for the Symbol after you place it. Just right
    Click on the symbol and Change the 'SpiceModel' Line to your subckt
    Not the same as editing the Attributes for the model file in the 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