Dismiss Notice
Join Physics Forums Today!
The friendliest, high quality science and math community on the planet! Everyone who loves science is here!

Is there vacuum tube models for LTspice?

  1. Jan 30, 2012 #1
    I know the default library of LTspice don't have vacuum tube model. Does anyone know where I can get one. If not, any other free spice program have vacuum tube models?

    The only one I find so far is:

    http://www.duncanamps.com/technical/ltspice.html

    I tried to follow the instruction and got lost.

    Thanks

    Alan
     
    Last edited: Jan 30, 2012
  2. jcsd
  3. Feb 1, 2012 #2

    vk6kro

    User Avatar
    Science Advisor

    View attachment 6AU6.zip

    Alan,

    There are some models of vacuum tubes on the Yahoo Group

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

    You may have to be a member to view the files, but this is free and fairly simple, I recall.

    Note that Europeans (and Australians) referred to these as "valves", so search for those as well.

    You need an ASY file and an INC file which you download and put in the "Special Functions" directory of LTSpice. (you can put them anywhere but this one makes it easy to find them.)
    c:\Program Files\LTC\LTspiceIV\lib\sym\SpecialFunctions\

    To use them, you can choose the diagram from the ASY file by going to the "Special Functions" components.
    Then you have to include a Spice directive (under "edit" on the main screen for LTSpice).
    You type .inc name-of-file
    Or you can just copy the whole contents of the INC file and paste it into the spice directive.
    This prints it on the screen but it works OK.

    I have attached a different type of file with a .CIR extension.
    It is just a text file so you can copy the test starting with "subckt" down to "end" and paste this in as a spice directive. Looks a bit messy on the screen, but it works.

    There is data for another tube in that file as well.



    Here is a subckt file for a 12ax7 (don't forget the first dot.)
    .SUBCKT 12AX7A P G K
    E1 2 0 VALUE={45+V(P,K)+95.43*V(G,K)}
    R1 2 0 1.0K
    Gp P K VALUE={1.147E-6*(PWR(V(2),1.5)+PWRS(V(2),1.5))/2}
    Cgk G K 1.6P
    Cgp G P 1.7P
    Cpk P K 0.46P
    .ENDS 12AX7A

    Here is one for a 6BM8 pentode:
    .SUBCKT 6BM8P A S G K
    *
    * Calculate contribution to cathode current
    *
    Eat at 0 VALUE={0.636*ATAN(V(A,K)/15)}
    Egs gs 0 VALUE={LIMIT{V(S,K)/7+V(G,K)*1.3+V(A,K)/700,0,1E6}}
    Egs2 gs2 0 VALUE={PWRS(V(gs),1.24)}
    Ecath cc 0 VALUE={V(gs2)*V(at)}
    *
    * Calculate anode current
    *
    Ga A K VALUE={3.45E-3*V(cc)}
    *
    * Calculate screen current
    *
    Escrn sc 0 VALUE={V(gs2)*(1.1-V(at))}
    Gs S K VALUE={3.7E-3*V(sc)*LIMIT{V(S,K),0,10}/10}
    *
    * Capacitances
    *
    Cg1 G K 9.6p
    Cak A K 9.3p
    Cg1a G A 0.35p

    .ENDS

    I find just pasting these into the Spice directive works well while the INC command gives lots of trouble. Probably me.

    Note that there are triode, pentode and tetrode symbols under "MISC" in the components drawer. The 6BM8 works if you choose the tetrode symbol and the above Spice directive for the 6BM8P.
    You have to rename the symbol from "tetrode" to "6BM8P" to match the Spice directive.

    These are as much fun as shampooing cats, so lots of luck.
     
    Last edited: Feb 1, 2012
  4. Feb 1, 2012 #3
    Thanks, I'll work on this soon.

    Alan
     
Know someone interested in this topic? Share this thread via Reddit, Google+, Twitter, or Facebook




Similar Discussions: Is there vacuum tube models for LTspice?
Loading...