Connect with us

Help with LTspice

Discussion in 'Electronic Design' started by viking, Sep 16, 2007.

Scroll to continue with content
  1. viking

    viking Guest

    Probably everyone but me knows how to do this but how do you step the
    frequency of an AC source while doing a transient analysis, for
    example perform a transient analysis at 1MHz steps from 1 to 10MHz.
    Thanks
    Rob
     
  2. ----- Original Message -----
    From: "viking" <>
    Newsgroups: sci.electronics.design
    Sent: Sunday, September 16, 2007 1:19 PM
    Subject: Help with LTspice


    Hello Rob,

    What means "steps"?
    What's the type of the signal? (sine?)

    Three chances with .TRAN
    ------------------------
    One simulation run: continuous frequency sweep
    One simulation run: stepped frequency 1Mhz, 2MHz, ..
    Multiple simulation runs: .step command

    If you simply want the frequency response of
    a linear system, the .AC comamnd should be used.

    Which case fits your requirement?
    Can you tell more what you try to simulate?
    It will help to give the right answer.

    Best regards,
    Helmut

    LTspice user group
    http://tech.groups.yahoo.com/group/LTspice/
     
  3. viking

    viking Guest

    Hello Helmut,
    Sorry not giving full details.
    I have .tran 0.01 and an Sine source AC 1
    I want to run multiple simulations (plotted on the same graph) for
    either a given list of frequencies or continous sweep.
    I've tried every combination of syntax using the .STEP comand without
    success (usually get syntax error).
    For eqample the simple set-up below:-

    Version 4
    SHEET 1 880 680
    WIRE 128 160 128 112
    WIRE 128 272 128 240
    FLAG 128 272 0
    FLAG 128 112 OUT
    SYMBOL voltage 128 144 R0
    WINDOW 3 73 57 Left 0
    WINDOW 123 24 132 Left 0
    WINDOW 39 0 0 Left 0
    SYMATTR InstName V1
    SYMATTR Value SINE(0 0.01 1000000)
    SYMATTR Value2 AC 1
    TEXT -2 506 Left 0 !.tran 0.01

    So this gives the result for 1MHz, but how to have it repeat the run
    for 2MHz..etc, plotted on the same graph.

    Thanks
    Rob
     
  4. Hello Rob,

    The curly braces {} are needed for values
    defined in .step commands.

    I have made two sweeper examples for you.

    Best regards,
    Helmut


    Maybe the news reader breaks long TEXT-lines.
    Please repir it if necessary.

    TEXT ....
    ,,,,

    TEXT ....,,,,



    Stepepd sweep, Test1.asc
    ------------------------

    Version 4
    SHEET 1 880 680
    WIRE 128 112 128 64
    WIRE 416 112 128 112
    WIRE 544 112 496 112
    WIRE 608 112 544 112
    WIRE 544 144 544 112
    WIRE 128 160 128 112
    WIRE 128 272 128 240
    WIRE 544 272 544 208
    FLAG 128 272 0
    FLAG 128 64 OUT
    FLAG 544 272 0
    FLAG 608 112 filt
    IOPIN 608 112 Out
    SYMBOL voltage 128 144 R0
    WINDOW 3 73 57 Left 0
    WINDOW 123 24 132 Left 0
    WINDOW 39 0 0 Left 0
    SYMATTR Value SINE(0 0.01 {freq1})
    SYMATTR Value2 AC 1
    SYMATTR InstName V1
    SYMBOL res 400 128 R270
    WINDOW 0 32 56 VTop 0
    WINDOW 3 0 56 VBottom 0
    SYMATTR InstName R1
    SYMATTR Value 1k
    SYMBOL cap 528 144 R0
    SYMATTR InstName C1
    SYMATTR Value 100p
    TEXT 8 -72 Left 0 !.tran 100u
    TEXT 16 -192 Left 0 !.step param freq1 1e6 5e6 2e6
    TEXT 8 -40 Left 0 !.options plotwinsize=0
    TEXT 16 -160 Left 0 ;.step param freq1 list 1e6 2e6 5e6 10e6




    Continuous sweep, Test2.asc
    ---------------------------

    Version 4
    SHEET 1 916 680
    WIRE -208 -128 -224 -128
    WIRE -224 -96 -224 -128
    WIRE -224 16 -224 -16
    WIRE 224 80 192 80
    WIRE 224 112 224 80
    WIRE 224 112 112 112
    WIRE 272 112 224 112
    WIRE 400 112 352 112
    WIRE 464 112 400 112
    WIRE -224 128 -256 128
    WIRE 112 144 112 112
    WIRE 400 144 400 112
    WIRE 64 160 -80 160
    WIRE 64 240 64 208
    WIRE 112 240 112 224
    WIRE 400 240 400 208
    FLAG 192 80 in
    FLAG 400 240 0
    FLAG 464 112 filt
    IOPIN 464 112 Out
    FLAG 64 240 0
    FLAG 112 240 0
    FLAG -224 16 0
    FLAG -208 -128 vfmod
    FLAG -256 128 vfmod
    SYMBOL res 256 128 R270
    WINDOW 0 32 56 VTop 0
    WINDOW 3 0 56 VBottom 0
    SYMATTR InstName R1
    SYMATTR Value 1k
    SYMBOL cap 384 144 R0
    SYMATTR InstName C1
    SYMATTR Value 100p
    SYMBOL SpecialFunctions\\modulate -224 128 R0
    WINDOW 123 -101 123 Left 0
    SYMATTR Value2 space=1 mark=10e6
    SYMATTR InstName A1
    SYMBOL e 112 128 R0
    SYMATTR InstName E1
    SYMATTR Value 0.01
    SYMBOL voltage -224 -112 R0
    WINDOW 123 0 0 Left 0
    WINDOW 39 0 0 Left 0
    SYMATTR InstName V1
    SYMATTR Value PWL(0 0.1 1m 1)
    TEXT 8 -72 Left 0 !.tran 1m
    TEXT 16 -192 Left 0 !.param fstart=1e6 fstop=5e6 TSWEEP=100u
    TEXT 8 -40 Left 0 !.options plotwinsize=0
    TEXT 16 -160 Left 0 ;.step param freq1 list 1e6 2e6 5e6 10e6
    TEXT 160 192 Left 0 ;gain
     
  5. Jim Thompson

    Jim Thompson Guest

    [snip]

    AC is NOT the same as SINE.

    You can't run a .AC simultaneously with a .TRAN

    ...Jim Thompson
     
  6. viking

    viking Guest

    Hello Helmut
    Thanks for that. The first example is the sort of thing I'm after.
    But the example you give crashes the application when run!
    I modified it at got the following to work:-

    Version 4
    SHEET 1 880 680
    WIRE 128 112 128 64
    WIRE 416 112 128 112
    WIRE 544 112 496 112
    WIRE 608 112 544 112
    WIRE 544 144 544 112
    WIRE 128 160 128 112
    WIRE 128 272 128 240
    WIRE 544 272 544 208
    FLAG 128 272 0
    FLAG 128 64 OUT
    FLAG 544 272 0
    FLAG 608 112 filt
    IOPIN 608 112 Out
    SYMBOL voltage 128 144 R0
    WINDOW 3 73 57 Left 0
    WINDOW 123 24 132 Left 0
    WINDOW 39 0 0 Left 0
    SYMATTR Value SINE(0 0.01 {freq1} 0 0 0 100)
    SYMATTR Value2 AC 1
    SYMATTR InstName V1
    SYMBOL res 400 128 R270
    WINDOW 0 32 56 VTop 0
    WINDOW 3 0 56 VBottom 0
    SYMATTR InstName R1
    SYMATTR Value 100k
    SYMBOL cap 528 144 R0
    SYMATTR InstName C1
    SYMATTR Value 10n
    TEXT 224 16 Left 0 !.tran 0.01
    TEXT 216 -16 Left 0 !.step param freq1 list 1000 2000 3000

    But you only have to change some parameters slightly for it to fall
    over, for example .trans 0.1 or add some more fequencies or use 1e6
    instead of 1000000.

    Rob
     
  7. viking

    viking Guest

    Hello Helmut, thakns for that.
    The first example is what I'm after, but it crashes when run. I
    modified it to that shown below and it now runs:-

    Version 4
    SHEET 1 880 680
    WIRE 128 112 128 64
    WIRE 416 112 128 112
    WIRE 544 112 496 112
    WIRE 608 112 544 112
    WIRE 544 144 544 112
    WIRE 128 160 128 112
    WIRE 128 272 128 240
    WIRE 544 272 544 208
    FLAG 128 272 0
    FLAG 128 64 OUT
    FLAG 544 272 0
    FLAG 608 112 filt
    IOPIN 608 112 Out
    SYMBOL voltage 128 144 R0
    WINDOW 3 73 57 Left 0
    WINDOW 123 24 132 Left 0
    WINDOW 39 0 0 Left 0
    SYMATTR Value SINE(0 0.01 {freq1} 0 0 0 100)
    SYMATTR Value2 AC 1
    SYMATTR InstName V1
    SYMBOL res 400 128 R270
    WINDOW 0 32 56 VTop 0
    WINDOW 3 0 56 VBottom 0
    SYMATTR InstName R1
    SYMATTR Value 100k
    SYMBOL cap 528 144 R0
    SYMATTR InstName C1
    SYMATTR Value 10n
    TEXT 224 16 Left 0 !.tran 0.01
    TEXT 216 -16 Left 0 !.step param freq1 list 1000 2000 3000

    But you only have to change a parameter slightly for it to crash, for
    example .tran 0.1 or add some more frequency steps.

    Rob
     

  8. Hello Rob,

    I had reported a similar problem with another circuit
    already to Mike this afternoon.
    I am sure there will be a fix latest until tomorrow.
    Sorry for this problem with the version 2.21m.
    I will reply as soon as a new version is available.
    If you need a previous version (e.g. 2.21f) of
    scad3.exe without this bug, you can download it from
    the Yahoo group or you send me your email address and
    I will mail it to you. It's 2MB in a zip-file.

    http://tech.groups.yahoo.com/group/LTspice/files/

    Best regards,
    Helmut
     
  9. viking

    viking Guest

    Hello Helmut,
    Thanks for taking the time to help. I will wait for the fix to come
    out.
    I will not be able to get back to the project I was using it on untill
    next week.
    Thanks again.
    Rob
     
  10. Hello Helmut,
    Hello Rob

    This bug is fixed now.
    There is a new version of LTspice (2.21n) available for download.
    Please upgrade.

    Btw, are you aware that this bug has been fixed on Sunday? :)

    Best regards,
    Helmut
     
  11. viking

    viking Guest

    Hello Helmut,
    Just downloaded lates version, works a treat.
    Thanks for taking the time to help out.
    Regards
    Rob
     
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

-