Dismiss Notice
Join Physics Forums Today!
The friendliest, high quality science and math community on the planet! Everyone who loves science is here!

Mis-matched pin count error in ltspice

Tags:
  1. Feb 15, 2017 #1
    Hi. I have a simple circuit with a third-part model. As far as I can tell using info from the internet I have everything correct, but I still get this problem. Please help me clear this log-jam, thanks!
     
  2. jcsd
  3. Feb 15, 2017 #2

    berkeman

    User Avatar

    Staff: Mentor

    Welcome to the PF.

    Can you upload a screenshot of your schematic? And maybe your SPICE deck for the model?
     
  4. Feb 15, 2017 #3
    Thanks for the quick reply! Here is as much as I can find you might need.
    show.php?id=112565.jpg
    show.php?id=112566.jpg show.php?id=112567.jpg
    Code (Text):

    * VCA810
    *****************************************************************************
    * (C) Copyright 2012 Texas Instruments Incorporated. All rights reserved.                                          
    *****************************************************************************
    ** This model is designed as an aid for customers of Texas Instruments.
    ** TI and its licensors and suppliers make no warranties, either expressed
    ** or implied, with respect to this model, including the warranties of
    ** merchantability or fitness for a particular purpose.  The model is
    ** provided solely on an "as is" basis.  The entire risk as to its quality
    ** and performance is with the customer.
    *****************************************************************************
    *
    ** Released by: WEBENCH(R) Design Center, Texas Instruments Inc.
    * Part: VCA810
    * Date: 01/15/2014
    * Model Type: All In One
    * Simulator: Pspice
    * Simulator Version: v16.2.0
    * EVM Order Number: N/A
    * EVM Users Guide: N/A
    * Datasheet: SBOS275F –JUNE 2003–REVISED DECEMBER 2010
    *
    * Model Version: 2.0
    *
    *****************************************************************************
    *
    * Updates:
    *
    * Version 1.0 : "VCA810 VOLTAGE CONTROLLED AMPLIFIER "MACROMODEL" SUBCIRCUIT
    *               CREATED 7/30/04 RRS"
    *               Release to Web
    * Version 2.0 : Update header text
    *
    *****************************************************************************
    * Notes:
    * 1. The model still missing dc and noise to be added later
    *****************************************************************************
    *
    * CONNECTIONS:     NON-INVERTING INPUT
    *                   |  GROUND
    *                   |  |  GAIN CONTROL, VC
    *                   |  |  |  OUTPUT
    *                   |  |  |  |  POSITIVE SUPPLY VOLTAGE
    *                   |  |  |  |  |  NEGATIVE SUPPLY VOLTAGE
    *                   |  |  |  |  |  |  INVERTING INPUT
    *                   |  |  |  |  |  |  |
    .SUBCKT  VCA810/BB  1  2  3  5  6  7  8
    * CONTROL VOLTAGE
    Q1   7   3  13  P
    C1   3   7  1E-12
    Q2   7   2  13  P
    I1   6  13  384E-6
    Q3  10  11  7  N
    R2   6  10  2
    E1  11   7  POLY(1) (3,0) 0.45  -0.11911
    G3  12   0  POLY(1) (10,6) 0 1
    R3  12   0  139
    C3  12   0  1.145E-9
    G1   6   7  POLY(1) (6,10) 13.5102E-3 -0.489
    G2   0   7  POLY(1) (6,10) 1.7958E-3 2.939E-3
    * INPUT STAGE
    Q01  20   1  26  N
    C01   1   0  1E-12
    Q02  21   8  26  N
    C02   8   0  1E-12
    R01  20  27  1E3
    D01  29  27  DX
    D03   6  29  DX
    R02  21  28  1E3
    D02  24  28  DX
    D04   6  24  DX
    IS   26   7  2.32E-3
    * GAIN STAGE 1
    R31  31   0  1E6
    G31  31   0  POLY(2) (8,1) (12,0) 0 0 0 0 1.1E-6 0
    * GAIN STAGE 2
    R41  41  44  20E3
    C41  41  44  230.25E-15
    G41  41  44  0  31  1E-3
    D41  41  43  DX
    E41  44  43  POLY(1) (3,0) 100.2 14.87
    R42  41  45  20E3
    C42  41  45  230.25E-15
    G42  41  45  0  31  1E-3
    D42  42  41  DX
    E42  42  45  POLY(1)  (3,0) 100.2 14.87
    E43  44   0  6  0  20
    E44   0  45  0  7  20
    * OUTPUT STAGE
    E51  55  0 41 0 50E-3
    D53  55  51  DX
    D54  52  55  DX
    D55   6  53  DX
    D56   6  54  DX
    D57   7  53  DZ
    D58   7  54  DZ
    G54  53   7  5  55  50E-3
    G53  54   7  55  5  50E-3
    V53  51   5  0.1833
    V54   5  52  0.1833
    G51   5   6  6  55  50E-3
    G52   7   5  55   7  50E-3
    R53   6   5  20
    R54   7   5  20
    .MODEL N NPN (IS=1E-12 BF=193)
    .MODEL P PNP (IS=1E-12 BF=96)
    .MODEL  DX  D(IS=1E-15 BV=200)
    .MODEL  DZ  D(IS=1E-15 BV=50)
    .ENDS
    *$
     
    Last edited by a moderator: Feb 15, 2017
  5. Feb 15, 2017 #4

    berkeman

    User Avatar

    Staff: Mentor

    When do you get the mismatched pin count error? When you try to run a DC or AC analysis? Does it specifically say it is for that device?

    Can you run the rest of the circuit without the 2nd amp and there are no problems? How about just the 2nd amp by itself with its circuitry?
     
  6. Feb 15, 2017 #5

    berkeman

    User Avatar

    Staff: Mentor

    BTW, pin 4 seems to be missing in the part description. Is it a No-Connect pin on the actual part?
     
  7. Feb 15, 2017 #6
    Hi Berkeman, thanks for your help.
    I had no problem with the first amp by itself, then I added in this third-party model.
    I assume since the LTspice model has the same number of pins as the definition it shouldn't be a problem since it is so common. I have not looked at the actual part but I assume it must be an nc.
    AC and DC analysis both give the same error.
    What is odd is that ltspice says the symbol has too many pins. Where?
    I added a dummy #4 pin in the symbol and and inserted the same in the spice model; it runs! Thanks for hint.
    In the absence of true knowledge I can live with a workaround.
    Here is the error popup:
    show.php?id=112574.jpg
     
  8. Feb 15, 2017 #7

    berkeman

    User Avatar

    Staff: Mentor

    Very cool -- good idea to try adding a dummy pin. Strange that the error occurred, but I agree that you've found a good workaround.
     
  9. Feb 15, 2017 #8
    This is several times now I have fixed an LTspice problem by making sure all the pins were tied to something. Pins that are allowed to float in reality need to be fixed for the sim to run in my last problem. This 'too many pins' error sort of falls into the same category: pins, pins, it's all about pins!
     
  10. Feb 23, 2017 #9

    Baluncore

    User Avatar
    Science Advisor

    Spice is nodes, it's all about nodes.

    A subcircuit in spice is like a subroutine or a function in a programming language. The technical term for the number of parameters passed is “arity”.

    The node numbers of the signals connected to a subcircuit are passed as parameters. When the arity differs between the model.sym and the model.sub then LTspice can tell you, but it can't fix it. You need to know that something is very wrong and you need to fix it.

    When you import a foreign spice model.sub to LTspice, the arity may be the same, but the order of the nodes may be different. LTspice can tell you if the arity is wrong but it cannot tell you if the parameter order is different. That most often happens when five terminal op-amp models are imported from other manufacturers libraries.

    The other trap to watch out for when importing subcircuits is identifying connections to ground inside the model that do not have an external node such as Com or Vss. You must work out why they are there and if they are sensible.
     
  11. Feb 23, 2017 #10
    Baluncore, that arity requirement must also apply to missing numbers in a pin sequence, since everything else matched in my previous problem with the missing pin 4.
    thanks for you input
    Matt
     
Know someone interested in this topic? Share this thread via Reddit, Google+, Twitter, or Facebook

Have something to add?
Draft saved Draft deleted



Similar Discussions: Mis-matched pin count error in ltspice
Loading...