LTSpice: How do make a Schmitt oscillator run?

Discussion in 'CAD' started by Joerg, Sep 16, 2008.

  1. Joerg

    Joerg Guest

    Ok, simple circuit: Schmitt inverter, 10K resistor from output to input,
    1000pF capacitor from input to ground. Vh set to about 20% of Vhigh.
    Should happily oscillate but I get the error message "Time step too
    small". Also there is a noted dip in voltage down to about 80%,
    something which should even be possible with a digital behavioral device.

    What gives? How can I fix that and make it run? Does it need some kind
    of kicker?
    Joerg, Sep 16, 2008
    1. Advertisements

  2. Hallo Joerg,

    I don't know what you did wrong.
    Have you set the trigger levels vt and vh?

    hysteresis: vh
    trigger levels:
    v1 = vt+vh
    v2 = vt-vh

    Example: Right-mouse-click on teh schmitt device.
    Vhigh=5 Vt=2.5 Vh=1


    Version 4
    SHEET 1 880 680
    WIRE 144 0 96 0
    WIRE 288 0 224 0
    WIRE 96 96 96 0
    WIRE 128 96 96 96
    WIRE 176 96 128 96
    WIRE 288 96 288 0
    WIRE 288 96 240 96
    WIRE 320 96 288 96
    WIRE 96 112 96 96
    WIRE 96 192 96 176
    FLAG 96 192 0
    FLAG 320 96 out
    FLAG 128 96 rc
    SYMBOL Digital\\schmtinv 176 32 R0
    SYMATTR InstName A2
    SYMATTR Value2 Vhigh=5 Vt=2.5 Vh=1
    SYMATTR SpiceLine Td=5n
    SYMBOL cap 80 112 R0
    SYMATTR InstName C1
    SYMATTR Value 1n
    SYMBOL res 128 16 R270
    WINDOW 0 32 56 VTop 0
    WINDOW 3 0 56 VBottom 0
    SYMATTR InstName R1
    SYMATTR Value 10k
    TEXT 80 -104 Left 0 !.tran 0 100u 0 100n
    Helmut Sennewald, Sep 16, 2008
    1. Advertisements

  3. Joerg

    Joerg Guest

    Thanks, Helmut. I did have everything in there except td since it wasn't
    mentioned in the LTSpice manual. That did it. But I still have a weak
    output, dips about 3V from the rails with Vhigh=12 with some serious
    inductive load and 2ohms in series. Somehow that doesn't look normal. Do
    they have a finite output current capability?

    When I tried to open your file I got a syntax error.
    Joerg, Sep 16, 2008

  4. Hello Joerg,

    I copied my attached circuit into a file "osc.asc" and it worked.
    You should copy the text from line "Version 4" to the end.
    (The line "Version 4" is already part of the schematic file osc.asc.)

    Version 4
    TEXT 80 -104 Left 0 !.tran 0 100u 0 100n

    I think it has 1 Ohm output resistance.
    Please add an E-source with gain 1 at the ouput to get a low output

    Best regards,
    Helmut Sennewald, Sep 16, 2008
  5. Joerg

    Joerg Guest

    That is what I tried.

    Aha! Thanks. That explains it.

    Well, a 1ohm Z Out is pretty much what my final driver will have so
    it'll be ok this time.

    Thanks for your help, Helmut.
    Joerg, Sep 16, 2008

  6. Hello,

    "ref" is the threshold for normal digital devices like AND and OR.
    If you don't specify "ref", it's (vhigh+vlow)/2

    The threshold for Schmitt trigger devices is "vt" and "vh", but not "ref".

    Helmut Sennewald, Sep 17, 2008
  7. Joerg


    Jul 25, 2010
    Likes Received:
    schmit trigger oscelator. is there some kind of update that can fix all that?

    i was using the free trial of multisim and it's schmit trigger works normaly. but lt threw me.
    i tried t o uninstall it from xp pro sp3 in add/remove and it just blinkes. restarted and same..
    at least now i can try to rtemodel its schmit trigger. thanks.
    is there any other models that have to be altered t o make them do their functions?
    jonathanscottjames, Jul 25, 2010
  8. Joerg


    Jul 25, 2010
    Likes Received:
    i meant to say ltspice4.08 works but won't uninstall. reinstalling didn't help

    i meant to say ltspice4.08 works but won't uninstall. reinstalling didn't help
    jonathanscottjames, Jul 26, 2010
    1. Advertisements

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.