1. Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.
    Dismiss Notice

"Time step too small" error in LTspice.

Discussion in 'Circuit Simulation & PCB Design' started by Flyback, Feb 1, 2014.

  1. Flyback

    Flyback Well-Known Member

    Joined:
    Jan 5, 2007
    Messages:
    1,989
    Likes:
    34
    Hello,
    Do you know how I can get this simulation working?, it gives the above error.
     

    Attached Files:

  2. ericgibbs

    ericgibbs Well-Known Member Most Helpful Member

    Joined:
    Jan 4, 2007
    Messages:
    21,185
    Likes:
    644
    Location:
    Ex Yorks' Hants UK
    ONLINE
    hi,
    It work for me,
    Goto Tools/Control Panel,,, select Alternate NOT Normal
    E
     

    Attached Files:

  3. Flyback

    Flyback Well-Known Member

    Joined:
    Jan 5, 2007
    Messages:
    1,989
    Likes:
    34
    tried alternate 1 and 2, and runs for a bit but then stops and gives the error...I am using windows 8
     
  4. dave

    Dave New Member

    Joined:
    Jan 12, 1997
    Messages:
    -
    Likes:
    0


     
  5. ericgibbs

    ericgibbs Well-Known Member Most Helpful Member

    Joined:
    Jan 4, 2007
    Messages:
    21,185
    Likes:
    644
    Location:
    Ex Yorks' Hants UK
    ONLINE

    I am using XP Pro.

    You didnt add the TLV431_ti model to your file so I used my TL431, it should be the same.

    Could your TLV model be the problem.?
     

    Attached Files:

  6. Flyback

    Flyback Well-Known Member

    Joined:
    Jan 5, 2007
    Messages:
    1,989
    Likes:
    34
    The tlv431 model I used is from Helmut sennewald on the ltspice forum, as attached

    the model worked fine in other sims with less nodes.
     

    Attached Files:

  7. ericgibbs

    ericgibbs Well-Known Member Most Helpful Member

    Joined:
    Jan 4, 2007
    Messages:
    21,185
    Likes:
    644
    Location:
    Ex Yorks' Hants UK
    ONLINE
    hi,
    With your model and Trtol=1 it never solves the sim!, change Trtol = 7 [ on the same Tools window as 'Alternate]

    It runs slow but it will solve
    E

    EDIT:
    Sometimes it fails! There is a problem with your model
     

    Attached Files:

  8. Flyback

    Flyback Well-Known Member

    Joined:
    Jan 5, 2007
    Messages:
    1,989
    Likes:
    34
    trtol to 7 and it still doesnt work
     
  9. ronv

    ronv Well-Known Member Most Helpful Member

    Joined:
    May 30, 2010
    Messages:
    4,725
    Likes:
    488
    Location:
    Tucson, AZ. USA
    Try this spice directive.

    .options gmin=1e-10

    If not.

    **********************************************************************************
    * Model developed by Eugene Dvoskin "http://www.audio-perfection.com" 02/05/2012
    * This TL431 model has been developed from schematic in the datasheet
    * http://www.ti.com/lit/ds/symlink/tl431.pdf
    * It matches most of DC, AC, Transient, Stability and Noise performance of TI TL431
    * No attempts were made to cover Temperature dependences
    *********************************************************************************
    .SUBCKT TL431ED CATHODE ANODE REF
    Q1 CATHODE REF N005 QN_ED
    R4 N005 N009 3.28k
    R2 N009 N012 2.4k
    R3 N009 N010 7.2k
    Q2 N012 N012 ANODE QN_ED area=1.2
    Q3 N010 N012 N014 QN_ED area=2.2
    R1 N014 ANODE 800
    Q4 N003 N005 N006 QN_ED
    R5 N006 N011 4k
    Q5 N011 N010 ANODE QN_ED
    Q6 N004 N013 ANODE QN_ED area=0.5
    Q7 N003 N003 N001 QP_ED
    Q8 N004 N003 N002 QP_ED
    R7 CATHODE N001 800
    R8 CATHODE N002 800
    Q9 CATHODE N004 N007 QN_ED
    R9 N008 N007 150
    Q10 CATHODE N008 ANODE QN_ED area=5
    R10 N008 ANODE 10k
    Q11 N004 N004 REF QN_ED
    D1 ANODE N004 D_ED
    R6 N013 N012 1k
    D2 ANODE CATHODE D_ED
    C1 CATHODE N004 10p
    C2 N010 N011 20p
    .model QN_ED NPN(BF=140 Cje=1p Cjc=2p Rb=40 VAF=80 VAR=50 KF=3.2e-16 AF=1)
    .model QP_ED PNP(BF=60 Cje=1p Cjc=3p Rb=80 VAF=70 VAR=40)
    .MODEL D_ED D(Rs=5 CJ0=4.0p)
    .ends TL431ED
     
  10. ericgibbs

    ericgibbs Well-Known Member Most Helpful Member

    Joined:
    Jan 4, 2007
    Messages:
    21,185
    Likes:
    644
    Location:
    Ex Yorks' Hants UK
    ONLINE
    hi Flyback,
    This zip has all my LTS TL431 information.
    The asc file uses my TL431 model, it runs in LTS.
    E
     

    Attached Files:

  11. Flyback

    Flyback Well-Known Member

    Joined:
    Jan 5, 2007
    Messages:
    1,989
    Likes:
    34
    thanks, I should say though, that this is TLV431

    Thanks, but ".options gmin=1e-10" doesnt make it work.

    The really weird thing is that if I run the simulation with V1 set to 12V, the simulation runs fine
     
  12. alec_t

    alec_t Well-Known Member Most Helpful Member

    Joined:
    Jul 10, 2011
    Messages:
    9,253
    Likes:
    1,218
    Location:
    Cardiff, Wales
    I often get that error message with sims. Sometimes the alternatesolver, or trtol, or gmin trick works; sometimes not. For reasons I haven't sussed, just changing a component value slightly can sometimes get it working. Schematics with inductors or high value caps seem to be the main types which trigger the error.
    There's an option to select the maximum time step; shame there's no way to set the minimum :(.
     
  13. Flyback

    Flyback Well-Known Member

    Joined:
    Jan 5, 2007
    Messages:
    1,989
    Likes:
    34
    OK thanks all, you got me on the right track saying about the TLV431 model.....that was the problem,

    here they are on ltspice yahoo groups "analogspiceman" is telling it and giving solution...I used his model...
    I changed to his tlv431as and it is fine......................
     
  14. ericgibbs

    ericgibbs Well-Known Member Most Helpful Member

    Joined:
    Jan 4, 2007
    Messages:
    21,185
    Likes:
    644
    Location:
    Ex Yorks' Hants UK
    ONLINE
    hi,
    Thats good news, when you have a minute please post the TLV431AS data.
    E
     
  15. Flyback

    Flyback Well-Known Member

    Joined:
    Jan 5, 2007
    Messages:
    1,989
    Likes:
    34
    ok
     

    Attached Files:

  16. ericgibbs

    ericgibbs Well-Known Member Most Helpful Member

    Joined:
    Jan 4, 2007
    Messages:
    21,185
    Likes:
    644
    Location:
    Ex Yorks' Hants UK
    ONLINE
    Got it, thanks.;)
     
  17. eTech

    eTech Active Member

    Joined:
    Apr 25, 2012
    Messages:
    561
    Likes:
    43
    Hi

    I tried your schematic in LTSpice. It failed with "Timestep too small"

    1. The TLV431.asy symbol attributes are incorrect. The only attibutes values should be:
    Prefix=X
    Value = TLV431
    Modelfile = tlv431.lib

    all others should be blank (except description if you like)
    Once I did this I had to remove and replace all TLV431's in the schematic.

    2. I was able to run the sim longer if I used this option:

    .options cshunt=1e-15

    not good..

    I would start by removing all the serial resistance values from all caps..
     

Share This Page