Connect with us

LTSpice newbie: simple model won't analyze

Discussion in 'CAD' started by Walter Harley, Apr 23, 2004.

Scroll to continue with content
  1. I'm hoping someone here can educate me on how to work through a simple
    problem in LTSpice. (I'll also try the Yahoo group, but I'm having troubles
    with that web page just now.)

    I have a simple circuit with two NOR gates, a resistor, and a capacitor.
    (Some of you might recognize it from a recent s.e.d posting.) I've appended
    the LTSpice .asc contents below. When I try simulating it, I get this
    error:
    "Analysis: Timestep too small; initial timepoint: trouble with
    or-instance a1".

    None of the obvious options on the simulation command seem to make any
    difference. One possibility is that I'm not using the OR gate correctly; per
    the online help, I'm leaving unused inputs unconnected. But I also tried
    grounding the unused inputs, and that didn't seem to make much difference.

    So, what do I need to do to get this to simulate successfully?


    Version 4
    SHEET 1 880 680
    WIRE 64 208 96 208
    WIRE 160 208 208 208
    WIRE 208 160 208 208
    WIRE 208 208 256 208
    WIRE 320 256 352 256
    WIRE 352 256 352 176
    WIRE 352 48 208 48
    WIRE 208 48 208 80
    WIRE 208 48 -32 48
    WIRE -32 48 -32 160
    WIRE -32 160 0 160
    WIRE 352 176 352 48
    WIRE 16 224 16 256
    WIRE 272 272 272 304
    FLAG 352 176 Vo
    FLAG 16 256 0
    FLAG 272 304 0
    SYMBOL Digital\\or 32 128 R0
    SYMATTR InstName A1
    SYMBOL Digital\\or 288 176 R0
    SYMATTR InstName A2
    SYMBOL cap 160 192 R90
    WINDOW 0 0 32 VBottom 0
    WINDOW 3 32 32 VTop 0
    SYMATTR InstName C1
    SYMATTR Value 1µF
    SYMBOL res 192 64 R0
    SYMATTR InstName R1
    SYMATTR Value 1k
    TEXT 64 288 Left 0 !.tran 10ms
     
  2. The problem is that those gates have no delay by default.
    Hence, the circuit sees a race condition. Right click on
    on of the Gate, and add a value of "Td=10n" to give the
    gate a 10ns delay. Then your circuit has a solution.

    --Mike
     
  3. That works great! (Actually, with Td=10n on one gate, it took a long time
    to simulate; with Td=10n on one and Td=15n on the other, it was
    instantaneous.)

    Thanks for the quick answer.
     
  4. Hello Walter,
    thanks for this tipp with the different delay time td.
    I wouldn't believe it, if I hadn't tried it.

    The simulation of this circuit either stucks at a fixed level
    or breaks into a wrong high frequency oscillation when using
    an equal delay time(10n) for both OR-gates.
    The behavior depends on the choosen solver. It seems to be a
    problem of symmetry.

    I will mention this tipp in the LSPICE Yahoo group if I post
    something about digital parts in the future.

    Best Regards,
    Helmut
     
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

-