Connect with us

.TEMP in Spice for just one component.

Discussion in 'Electronic Design' started by Jamie, Jun 18, 2013.

Scroll to continue with content
  1. Jamie

    Jamie Guest

    how do I specify a different operating temperature for a specific
    component instead of it applying it to all?

    .TEMP -32 for example is for all the components, but I would
    like to specify that a DIODE is at like -100 C for example, while
    every one else is at 38c et..

  2. Fred Abse

    Fred Abse Guest

    Something like this:

    Ctrl-right click on the diode symbol to get the full edit box, where you can
    enter the {T} parameter.

    You can set T to whatever you want, or step it. It will override the
    global temperature for that component only.

    I'm not sure how good the provided models are. There aren't any with Tikf,
    Trs1, and Trs2 set, and the LTspice default for all those is zero.

    Version 4
    SHEET 1 880 680
    WIRE 240 32 48 32
    WIRE 240 48 240 32
    WIRE 48 96 48 32
    WIRE 240 176 240 128
    WIRE 48 272 48 176
    WIRE 144 272 48 272
    WIRE 240 272 240 240
    WIRE 240 272 144 272
    WIRE 144 288 144 272
    FLAG 144 288 0
    SYMBOL schottky 224 176 R0
    WINDOW 123 24 76 Left 2
    SYMATTR InstName D1
    SYMATTR Value 1N5819
    SYMATTR Description Diode
    SYMATTR Type diode
    SYMATTR Value2 temp={T}
    SYMBOL res 224 32 R0
    SYMATTR InstName R1
    SYMATTR Value 1k
    SYMBOL voltage 48 80 R0
    WINDOW 123 0 0 Left 2
    WINDOW 39 0 0 Left 2
    SYMATTR InstName V1
    SYMATTR Value 10
    TEXT 312 96 Left 2 !.step param T -100 150 5
    TEXT 312 120 Left 2 !.op

    "For a successful technology, reality must take precedence
    over public relations, for nature cannot be fooled."
    (Richard Feynman)
  3. Jamie

    Jamie Guest

    Ok, the optional menu allowed me to enter TEMP -32 in a
    spice line, which resolved that problem..

    I've been working on a noise problem that uses signal diodes
    and these diodes are subjected to cold temperatures. One diode
    gets a different temp than the other and I use these to form a

    The signal is pulsed and after applying this TEMP parameter I can
    now see where the possible problem is.

    It seems that the diode increases temperature at the junction that
    takes up 250 ms, according to spice, to level out. This changes
    the Vf during that time..

    So I shorten the pulse down to 10 ms and I don't see this any more.

    We'll have to apply this in real life to see if this helps. We are
    trying very hard not to use much for filtering so that we can maintain
    response time.

    It's possible Ltspice is giving me some bogus numbers, i've always been
    partial to bench testing over sims.

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