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

Ngspice to PSpice conversion

  1. Jun 1, 2012 #1
    Hi All,

    I have a piece of Ngspice code that I need to convert to PSpice. I feel it is a simple matter of syntax but I have so far failed to make it work.

    The code models a Memristor with thresholding ability (the fourth fundamental component along with resistors, capacitors, and inductors)

    The code is as follows:

    .subckt memristor plus minus PARAMS: Ron=1K Roff=10K Rinit=5K alpha=0 beta=1E13 Vt=4.6
    Bx 0 x I='(f1(V(plus)-V(minus))>0) && (V(x)<Roff) ? {f1(V(plus)-V(minus))}: (f1(V(plus)-V(minus))<0) && (V(x)>Ron) ? {f1(V(plus)-V(minus))}: {0}'
    Cx x 0 1 IC={Rinit}
    Rmem plus minus r={V(x)}
    .func f1(y)={beta*y+0.5*(alpha-beta)*(abs(y+Vt)-abs(y-Vt))}
    .ends


    The code explanation is as follows:
    - The memristive system is realized as a sub-circuit combining a behavioral resistor R, a current source ↑, and a capacitor C.
    - The second line of code (Bx ...) defines the current source with the current specified through ternary functions. (A ternary function is defined in the code as a ? b : c , which means ”IF a, THEN b, ELSE c” [17].) The purpose of these functions is to limit RM between Ron and Roff.
    - The third line of the code specifies the capacitor C (Cx ...) with an initial condition.
    - The fourth line (Rmem ...) defines the behavioral resistor whose resistance takes the same numerical value as the voltage across the capacitor.
    - The next line (.func ...) provides the function f according to Equation (not important here)


    If you can help me in any way that would be great!!

    Many thanks
    Captainkirk
     
  2. jcsd
  3. Jun 1, 2012 #2
    I can help you. But can you be a little more clear with simple circuit diagram and simple expressions?
     
  4. Jun 1, 2012 #3
    Hi there, thanks for replying.

    I've attached the circuit diagram as image.

    PLEASE NOTE - I dont need help with the Model, I just need help with syntax. Thats the code I gave in my first post just needs its syntax tweaked so it is compatible with Pspice.

    The research paper that I'm referring to states the following for the Spice model:

    "SPICE model: The memristive devices with threshold that we consider are those described by
    I = X-1VM
    X ̇ = (βVM +0.5(α−β)[|VM +Vt|−|VM −Vt|])

    where Vt is the threshold voltage, Ron and Roff are limiting values of the memristance RM ≡ X, and the θ-functions

    Note - These equations are represented in ngspice code I gave in my first post.

    - The important model parameters are the coefficients α and β that characterize the rate of memristance change at |VM|<Vt and |VM|>Vt , respectively.
    - These two coefficients define the slopes of the f (VM) curve below and above the threshold. When α = 0, the device state changes only if |VM| > Vt"

    Please let me know if this makes it clearer.

    I appreciate any help you can provide here!

    Many thanks again
    CaptainKirk
     
    Last edited: Jun 1, 2012
  5. Jun 1, 2012 #4
    attached file
     

    Attached Files:

  6. Jun 1, 2012 #5
    Captainkirk, I really did not try to understand the model. Actually I could not make out the ngspice syntax. I am working on it. You'll get your spice model after sometime.
     
  7. Jun 3, 2012 #6
    Kholdstare,

    see the ngspice-users forum (I am not allowed to give the link here).

    captainkirk is engaging at least three forums ...

    But is was nice just to get it up and running.

    Regards

    Holger
     
  8. Jun 3, 2012 #7
    Here's your PSpice macromodel as requested. To use it in your circuit just copy the "* memres ... begins" to "* memres ... ends" portion to your circuit and call the model using "X(ref) (node1) (node2) R_MEMR PARAMS: VCUT=(param) ALPHA=(param) BETA=(param)" device card.

    Code (Text):
    * memresistor model begins

    .MODEL SWD D IS=1E-16 N=0.001

    .FUNC GET_R1(ALPHA) {1/ALPHA}
    .FUNC GET_R2_R3(ALPHA,BETA) {1/ABS(BETA-ALPHA)}
    * ABS is given to prevent negative resistance

    .SUBCKT R_MEMR 1 2
    * Default parameters defined below
    + PARAMS: VCUT=1V ALPHA=0.1M BETA=0.2M
    R1 1 2 {GET_R1(ALPHA)}
    D2 1 3 SWD
    V2 3 4 {VCUT}
    R2 4 2 {GET_R2_R3(ALPHA,BETA)}
    D3 5 1 SWD
    V3 6 5 {VCUT}
    R3 6 2 {GET_R2_R3(ALPHA,BETA)}
    .ENDS

    * memresistor model ends

    *Test ckt

    * The voltage source
    V1 1 0 0Vdc
    * The memresistor (new parameters are passed as arguments)
    XMEMR_1 1 0 R_MEMR PARAMS: VCUT=4.6V ALPHA=0 BETA=1E-3

    .DC V1 -8 8 0.01
    .PROBE
    .END
    The test parameters I used are Vcut = 4.6V, alpha = 0, beta = 1e-3
    The test result is in the attachment.

    I simplified your expression as written below,
    I = a*V for |V| < Vt
    = a*V+(b-a)(V-Vt) for V>Vt
    = a*V+(b-a)(V+Vt) for V<Vt

    I could not model capacitance as you did not give its expression clearly.
     

    Attached Files:

  9. Jun 3, 2012 #8
    Sorry for the late. I had actually forgotten about it after your last post. Shows kinda lazy person I am. haha
     
  10. Jun 4, 2012 #9
    Kholdstare

    Thank you were much with your reply!!

    I can hardly call you lazy, after all you did come up with something very interesting.

    I'm very impressed with your model. Its is different from what I came up with but I still like the output graph that you attached!

    Thank you once again

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




Similar Discussions: Ngspice to PSpice conversion
  1. Pspice problem (Replies: 2)

  2. PSpice help (Replies: 1)

Loading...