+ Post New Thread
Results 1 to 13 of 13
  1. #1
    Full Member level 4
    Points: 1,256, Level: 8

    Join Date
    Aug 2016
    Posts
    235
    Helped
    2 / 2
    Points
    1,256
    Level
    8

    Can this spice model work with LTSPICEs' spice engine

    LTSPICEs' spice engine gives 'Only a level 9 bssoi can have 5 nodes' for nmos model FQP6N90C

    http://dpaste.com/0QDAYRJ

    https://www.fairchildsemi.com/datash...Q/FQP6N90C.pdf

    I don't write spice and am not familiar with it. Is the file beyond repair or is it a simple fix?

    •   AltAdvertisment

        
       

  2. #2
    Advanced Member level 1
    Points: 2,911, Level: 12

    Join Date
    Nov 2013
    Posts
    416
    Helped
    90 / 90
    Points
    2,911
    Level
    12

    Re: Can this spice model work with LTSPICEs' spice engine

    I think you added the thermal model of the spice subcircuit, those the 2 extra pins, probably it doesn't like it.
    Delete of the thermal model section maybe can solve it. Otherwise I don't know, the subcircuit should have 3 terminals, in the model the 2 1 3 nodes after the name of it.
    (strange that the MOS in the model have a width of 1.08m.... but probably good, if it is fairchild's model)
    "Try SCE to AUX." /John Aaron/


    1 members found this post helpful.

  3. #3
    Full Member level 4
    Points: 1,256, Level: 8

    Join Date
    Aug 2016
    Posts
    235
    Helped
    2 / 2
    Points
    1,256
    Level
    8

    Re: Can this spice model work with LTSPICEs' spice engine

    Quote Originally Posted by frankrose View Post
    I think you added the thermal model of the spice subcircuit, those the 2 extra pins, probably it doesn't like it.
    Delete of the thermal model section maybe can solve it. Otherwise I don't know, the subcircuit should have 3 terminals, in the model the 2 1 3 nodes after the name of it.
    (strange that the MOS in the model have a width of 1.08m.... but probably good, if it is fairchild's model)
    Removing the thermal part did nothing and using the thermal model gave same original issue.



  4. #4
    Advanced Member level 1
    Points: 2,911, Level: 12

    Join Date
    Nov 2013
    Posts
    416
    Helped
    90 / 90
    Points
    2,911
    Level
    12

    Re: Can this spice model work with LTSPICEs' spice engine

    Hmm... Maybe the model terminal names are different of the symbol. You should check that the symbol has the same 2 1 3 terminal names and are they refer to the correct pin. By the linked description: 2=drain, 1=gate, 3=source
    But the model description seems OK. LTSpice should handle it.
    "Try SCE to AUX." /John Aaron/


    1 members found this post helpful.

  5. #5
    Advanced Member level 5
    Points: 37,041, Level: 47

    Join Date
    Mar 2008
    Location
    USA
    Posts
    5,977
    Helped
    1732 / 1732
    Points
    37,041
    Level
    47

    Re: Can this spice model work with LTSPICEs' spice engine

    I vaguely recall having problems with LTSpice trying to use
    the geometry params, LTSpice being for discrete and IC use
    and not wanting the low down width, length, multiplier type
    params that pertain to free-for-all IC design. I think it's the
    geometry params after D G S B that are being complained
    about ("fifth node" when there are only 4, plus params).


    1 members found this post helpful.

    •   AltAdvertisment

        
       

  6. #6
    Super Moderator
    Points: 247,995, Level: 100
    Awards:
    1st Helpful Member

    Join Date
    Jan 2008
    Location
    Bochum, Germany
    Posts
    43,128
    Helped
    13122 / 13122
    Points
    247,995
    Level
    100

    Re: Can this spice model work with LTSPICEs' spice engine

    LTSPICEs' spice engine gives 'Only a level 9 bssoi can have 5 nodes' for nmos model FQP6N90C
    You don't show the model instantiation that gives the said error. Please ask complete questions.


    1 members found this post helpful.

    •   AltAdvertisment

        
       

  7. #7
    Full Member level 4
    Points: 1,256, Level: 8

    Join Date
    Aug 2016
    Posts
    235
    Helped
    2 / 2
    Points
    1,256
    Level
    8

    Re: Can this spice model work with LTSPICEs' spice engine

    Quote Originally Posted by FvM View Post
    You don't show the model instantiation that gives the said error. Please ask complete questions.
    You probably meant the circuit which gives the error.

    issue.zip



  8. #8
    Advanced Member level 1
    Points: 2,911, Level: 12

    Join Date
    Nov 2013
    Posts
    416
    Helped
    90 / 90
    Points
    2,911
    Level
    12

    Re: Can this spice model work with LTSPICEs' spice engine

    I simulated a simple circuit with the above model and it works for me. There are quite good video tutorials about how to use a subcircuit model in LTSpice, I suggest to watch one.
    "Try SCE to AUX." /John Aaron/


    1 members found this post helpful.

  9. #9
    Full Member level 4
    Points: 1,256, Level: 8

    Join Date
    Aug 2016
    Posts
    235
    Helped
    2 / 2
    Points
    1,256
    Level
    8

    Re: Can this spice model work with LTSPICEs' spice engine

    I cannot get it to simulate maybe there is a particular video you recommend.



  10. #10
    Super Moderator
    Points: 247,995, Level: 100
    Awards:
    1st Helpful Member

    Join Date
    Jan 2008
    Location
    Bochum, Germany
    Posts
    43,128
    Helped
    13122 / 13122
    Points
    247,995
    Level
    100

    Re: Can this spice model work with LTSPICEs' spice engine

    You probably meant the circuit which gives the error.
    You didn't yet post CC-Source-MOSFET.asc



  11. #11
    Full Member level 4
    Points: 1,256, Level: 8

    Join Date
    Aug 2016
    Posts
    235
    Helped
    2 / 2
    Points
    1,256
    Level
    8

    Re: Can this spice model work with LTSPICEs' spice engine

    Quote Originally Posted by FvM View Post
    You didn't yet post CC-Source-MOSFET.asc
    I missed the actual circuit and included an error log instead. Here is the circuit.

    issue-circuit.zip



  12. #12
    Advanced Member level 1
    Points: 2,911, Level: 12

    Join Date
    Nov 2013
    Posts
    416
    Helped
    90 / 90
    Points
    2,911
    Level
    12

    Re: Can this spice model work with LTSPICEs' spice engine

    Quote Originally Posted by Zak28 View Post
    I cannot get it to simulate maybe there is a particular video you recommend.
    I recommend you to generate with LTspice a symbol for your sub-block:
    1, copy the spice model of the transistor in a mosModel.txt file to the same folder where your testbench (= the .asc file) is
    2, open with LTSpice the mosModel.txt file, and click with the right mouse mouse button on the highlighted name of the transistor (= FQPF6N90C). Choose "Create symbol", save this (The generated pins should be 1 2 3 = Gate Drain Source).
    3, open your testbench (= the .asc file), press F2 and add the FQPF6N90C symbol from the AutoGenerated directory, from the sym library.
    4, on your testbench place a spice directive (at the toolbar click on the .op), type in .include mosModel.txt
    5, be sure on your testbench the name of the symbol is the same as the name of the transistor in the mosModel.txt.
    6, run a simulation
    "Try SCE to AUX." /John Aaron/



    •   AltAdvertisment

        
       

  13. #13
    Super Moderator
    Points: 247,995, Level: 100
    Awards:
    1st Helpful Member

    Join Date
    Jan 2008
    Location
    Bochum, Germany
    Posts
    43,128
    Helped
    13122 / 13122
    Points
    247,995
    Level
    100

    Re: Can this spice model work with LTSPICEs' spice engine

    The fault is in not referencing the subcircuit model correctly.

    It should be done like below:

    Click image for larger version. 

Name:	sub.PNG 
Views:	2 
Size:	7.5 KB 
ID:	149360

    Doing so reveals that Ltspice doesn't like this model

    Error on line 808 : .model m1:bsim3 nmos (level=7 version=3.1 mobmod=3 capmod=2 paramchk=1 nqsmod=0 tox=970e-10 xj=1.4e-6 nch=1.7e17 ua=1.6e-9 u0=700 vsat=1.0e5 drout=3.0 pvag=5 delta=0.10 pscbe2=0 rsh=1.0e-3 pdiblc2=1e-7 vth0=4.10 voff=-0.1 nfactor=1.1 lint=5.90e-7 dlc=5.90e-7 fc=0.5 cgso=9.32e-10 cgsl=0 cgdo=8.65e-12 cgdl=9.23e-10 cj=0 cf=0 ckappa=0.13 kt1=-2.07 kt2=0 ua1=1.02e-10 nj=10 )
    * Unrecognized parameter "fc" -- ignored
    Warning: Pscbe2 = 0 is not positive.
    Warning: Pd = 0 is less than W.
    Warning: Ps = 0 is less than W.
    Direct Newton iteration for .op point succeeded.
    Commenting parameter FC removes the error, there are warnings, nevertheless the circuit achieves a reasonable operation point.



--[[ ]]--