Connect with us

LM317 Netlist To Device??

Discussion in 'Electronic Basics' started by Randy Gross, Nov 16, 2004.

Scroll to continue with content
  1. Randy Gross

    Randy Gross Guest

    Greetings,

    I'm having more than a problem creating this device, LM317, in
    CircuitMaker. When I load the "lm317.net" file into CM, I get this
    message: "No Spice Analysis Specified in: lm317.net". OK, so I pull up
    the spice data help screen and now I'm totally confused. I gathered
    that the " % " sign preceeds the designations but, how do I define it
    as a device?

    This is my first attempt at creating a device from a netlist so any
    guidance in this matter will go a long way in restoring my battered
    ego;-)

    I've included the LM317 Netlist for examination:

    *Netlist
    *LM317 TI voltage regulator - pin order: In, Adj, Out
    *TI adjustable voltage regulator pkg:TO-3
    ..SUBCKT LM317 1 2 3
    J1 1 3 4 JN
    Q2 5 5 6 QPL .1
    Q3 5 8 9 QNL .2
    Q4 8 5 7 QPL .1
    Q5 81 8 3 QNL .2
    Q6 3 81 10 QPL .2
    Q7 12 81 13 QNL .2
    Q8 10 5 11 QPL .2
    Q9 14 12 10 QPL .2
    Q10 16 5 17 QPL .2
    Q11 16 14 15 QNL .2
    Q12 3 20 16 QPL .2
    Q13 1 19 20 QNL .2
    Q14 19 5 18 QPL .2
    Q15 3 21 19 QPL .2
    Q16 21 22 16 QPL .2
    Q17 21 3 24 QNL .2
    Q18 22 22 16 QPL .2
    Q19 22 3 241 QNL 2
    Q20 3 25 16 QPL .2
    Q21 25 26 3 QNL .2
    Q22A 35 35 1 QPL 2
    Q22B 16 35 1 QPL 2
    Q23 35 16 30 QNL 2
    Q24A 27 40 29 QNL .2
    Q24B 27 40 28 QNL .2
    Q25 1 31 41 QNL 5
    Q26 1 41 32 QNL 50
    D1 3 4 DZ
    D2 33 1 DZ
    D3 29 34 DZ
    R1 1 6 310
    R2 1 7 310
    R3 1 11 190
    R4 1 17 82
    R5 1 18 5.6K
    R6 4 8 100K
    R7 8 81 130
    R8 10 12 12.4K
    R9 9 3 180
    R10 13 3 4.1K
    R11 14 3 5.8K
    R12 15 3 72
    R13 20 3 5.1K
    R14 2 24 12K
    R15 24 241 2.4K
    R16 16 25 6.7K
    R17 16 40 12K
    R18 30 41 130
    R19 16 31 370
    R20 26 27 13K
    R21 27 40 400
    R22 3 41 160
    R23 33 34 18K
    R24 28 29 160
    R25 28 32 3
    R26 32 3 .1
    C1 21 3 30PF
    C2 21 2 30PF
    C3 25 26 5PF
    CBS1 5 3 2PF
    CBS2 35 3 1PF
    CBS3 22 3 1PF
    ..MODEL JN NJF(BETA=1E-4 VTO=-7)
    ..MODEL DZ D(BV=6.3)
    ..MODEL QNL NPN(EG=1.22 BF=80 RB=100 CCS=1.5PF TF=.3NS TR=6NS CJE=2PF
    CJC=1PF VAF=100)
    ..MODEL QPL PNP(BF=40 RB=20 TF=.6NS TR=10NS CJE=1.5PF CJC=1PF VAF=50)
    ..ENDS LM317

    Randy
     
  2. Randy:

    for an example, look in C:\CM06\Models\MCEREGS.LIB

    There is already an LM317 which looks identical to the one you are
    trying to create.

    --
    Regards,
    Robert Monsen

    "Your Highness, I have no need of this hypothesis."
    - Pierre Laplace (1749-1827), to Napoleon,
    on why his works on celestial mechanics make no mention of God.
     
  3. I don't know a lot about CM, but a netlist is the spice netlist, not a
    model .subckt specification. You are obviously loading in what CM thinks
    is a complete spice netlist that has a full run specified in it. You
    need to look at the documentation to find out how to add an actual
    *model*. Your problem is that you don't yet know what is what in spice.
    A spice netlist tells spice how the circuit is constructed and what to
    do with it. A model is a only *part* of a final netlist.

    The convention for files with models are .lib, .mod, .sub. The
    conventions for spice netlists are .cir and .net.

    If it were SuperSpice, it would be a no-brainier. Just drag drop a
    model.lib to the main window. The model will show up in the docked list
    on the left. When you place it is will pop up a dialog allowing you to
    chose an existing symbol to attach to it, if it cant figure it out
    itself.

    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.
     
  4. Chaos Master

    Chaos Master Guest

    IIRC, CircuitMaker already has LM317 symbol/model. Otherwise, you must
    create a 'macro' element that refers to your model.

    Don't ask me how to do this -- I'm no more a CircuitMaker user.

    []s
    --
    Chaos Master®, posting from Brazil.
    "It's not what it seems, not what you think. No, I must be dreaming."

    http://marreka.no-ip.com | http://tinyurl.com/46vru
    http://renan182.no-ip.org | http://marreka.blogspot.com (in Portuguese)
     
  5. <snip>

    I'm not clear what you are trying to do. Is this possibly a learning
    exercise, trying to create a model from scratch, but deliberately
    choosing a model that already exists so that you can check the result?
    You don't say which version, but from your other thread I assume
    you're using CM 6. As Robert has said, the CM 6 library already
    contains an LM317, and it has the spec you have listed. But, as
    already pointed out, that is the 'model subcircuit data', not the
    'netlist'.
     
  6. Randy Gross

    Randy Gross Guest

    Yes Terry, this is/was a learning exercise. I found the LM317 in the
    ..lib file and incorporated it however, I did'nt learn anything about
    creating a model from scratch. There are two other devices in the
    LM317/LM301A regulator circuit (found in the LM317 datasheet) that CM6
    does not have a model of I could find in the LIBs':

    MJ4502 Transistor, 200W, 100V, 30A, TO-3
    and
    IN457 Diode (no data yet)

    If I had a walk-thru on this first attempt, I would understand the
    process. The CM6 help files are a little confusing without an example.

    Randy
     
  7. With CM, you can pick a component that is similar, and do an 'edit
    model' on it. For example, if you want to enter a model of a MJ4502
    transistor, you pick one that is similar, enter it into a schematic,
    then double click on it. That brings up a dialog. Select the 'edit'
    button, and an editor comes up that allows you to create a new model.
    Get the values out of the datasheet, and rename the model, and then you
    can pick it just like any other transistor.

    Same goes for diodes.

    Some of the models will just bring up a netlist editor. In that case,
    just replace the appropriate values in the netlist.

    --
    Regards,
    Robert Monsen

    "Your Highness, I have no need of this hypothesis."
    - Pierre Laplace (1749-1827), to Napoleon,
    on why his works on celestial mechanics make no mention of God.
     
  8. Randy Gross

    Randy Gross Guest

    This approach will suit my needs perfectly. Thanks Robert! I have one
    more question concerning the IN457 diode listed in the LM317/LM301A
    circuit on page 16 of the datasheet. I can't find any reference to
    this diode (National, Motorola, DigiKey, datasheet search, etc.) so
    there's no data to sub the device if it proves outdated. I'm starting
    to think the number may be incomplete or in err.
    Can anyone help.

    Randy
     
  9. CircuitMaker 1N457 (not IN457!) diode model:

    IS: Saturation current 28.40p
    RS: Ohmic resistance [0,] 2.100
    N: Emission coefficient 1.700
    TT: Transit-time [0,] 4.320u
    CJO: Zero-bias junction capacitance [0,] 10.60p
    VJ: Junction potential 750.0m
    M: Grading coefficient 333.0m
    EG: Activation energy 1.110
    XTI: Saturation-current temperature exponent 3.000
    KF: Flicker-noise coefficient 0.000
    AF: Flicker-noise exponent 1.000
    FC: Foward-bias depletion coefficient 500.0m
    BV: Reverse breakdown voltage 60.00
    IBV: Current at breakdown voltage 66.00n
    TNOM:paramameter measurement temperature 27.00
     
  10. Randy Gross

    Randy Gross Guest

    Thanks to every one of you for solutions to my problems. Now I can get
    this circuit up and running to study what's going on in it before I
    build.

    Randy
     
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

-