Connect with us

Lm13700 LTSpice Sim Help

Discussion in 'General Electronics Discussion' started by bobtech, May 8, 2017.

Scroll to continue with content
  1. bobtech

    bobtech

    10
    1
    Apr 14, 2017
    Hi guys,

    I'm having an issue simulating the LM13700 in LTSpice.... I have trawled through the net to no avail.

    It's a standard setup for the LM13700 from the data sheet (Square/Triangle VCO) and I have some initial conditions which can be seen in LTSpice, to help kick it into oscillation (it stays flat at 0V and -1.3V otherwise) .... and the output I get is below (only runs for a fraction of a micro second)

    any ideas on where to go with this, why doesn't it display the waveform for longer? I'm stumped..

    [​IMG]
     
  2. Alec_t

    Alec_t

    2,736
    725
    Jul 7, 2015
    Please post your .asc file here.
     
  3. bobtech

    bobtech

    10
    1
    Apr 14, 2017
    there was a small mistake in the original, where I hadn't connected the capacitor to ground....
    I've fixed it but now it doesn't do anything o_O

    I also attached the asc file.

    [​IMG]
     

    Attached Files:

  4. bobtech

    bobtech

    10
    1
    Apr 14, 2017
    update: although no errors show when I run the sim, when I check the error log, I do get this error... any ideas?


     
  5. bobtech

    bobtech

    10
    1
    Apr 14, 2017
    Ok, so taking the advice of the logfile, I skipped the.op point.... however I get a new problem...

    upload_2017-5-8_20-31-20.png

     
  6. Harald Kapp

    Harald Kapp Moderator Moderator

    9,548
    1,973
    Nov 17, 2011
  7. Alec_t

    Alec_t

    2,736
    725
    Jul 7, 2015
    Like you, I failed to get your sim of the VCO in the datasheet to run. However, it can be made to run with the following changes (I daresay other changes would work too):-
    1) Reduce V3 to 1V,
    2) Increase C1 to 100n,
    3) Add the directive ".options gmin=1e-7" to the schematic.
     
  8. bobtech

    bobtech

    10
    1
    Apr 14, 2017
    Sorry, the model is take from the Texas instruments site directly, and loaded into LTSpice

    Here vvvvvv
    http://www.ti.com/product/LM13700/toolssoftware

    would the 1e-7 not give false results? (I remember reading somewhere not to really go past 1e-9)
     
  9. Harald Kapp

    Harald Kapp Moderator Moderator

    9,548
    1,973
    Nov 17, 2011
    Better some error with 1e-7 than no simulation at all with 1e-9.
    As with all simulations you have to take the result with a grain of salt anyway. The simulation can be only as good as the models used and who guarantees the model of the amplifier is as accurate as you expect?

    My personal stance is that the simulation is only there to verify there's no fatal flaw in the design calculations. A prototype will show the real world behavior much better than any simulation, including hard to simulate parameters such as e.g. noise, PCB Layout parasitics etc.
     
  10. eetech00

    eetech00

    95
    8
    Nov 17, 2014
    Hi

    The input offset current is modeled with an F device poly which doesn't converge very well.

    Change the following in the subcircuit definition:

    IS:
    F1 4 3 POLY(1) V6 1E-10 5.129E-2 -1.189E4 1.123E9

    Change to:
    *F1 4 3 POLY(1) V6 1E-10 5.129E-2 -1.189E4 1.123E9 <--comment this out
    B1 4 3 I=If(V(11)>1.4v,100nA,0)

    eT
     
    Harald Kapp likes this.
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

-