[SOLVED] problem with obtaining memristor I-V characteristic in LTSPICE

[fuadfadz]

Has anyone used a spice model of memristor? I am trying to use the model proposed in BIOLEK's paper (https://www.radioeng.cz/fulltexts/2009/09_02_210_214.pdf) in LTspice.

* HP Memristor SPICE Model
* For Transient Analysis only
* created by Zdenek and Dalibor Biolek
**************************
* Ron, Roff - Resistance in ON / OFF States
* Rinit - Resistance at T=0
* D - Width of the thin film
* uv - Migration coefficient
* p - Parameter of the WINDOW-function
* for modeling nonlinear boundary conditions
* x - W/D Ratio, W is the actual width
* of the doped area (from 0 to D)
*
.SUBCKT memristor Plus Minus PARAMS:
+ Ron=100 Roff=16K Rinit=11K D=10N uv=10F p=10
***********************************************
* DIFFERENTIAL EQUATION MODELING *
***********************************************
Gx 0 x value={ I(Emem)*uv*Ron/D**2*f(V(x),p)}
Cx x 0 1 IC={(Roff-Rinit)/(Roff-Ron)}
Raux x 0 1T
* RESISTIVE PORT OF THE MEMRISTOR *
*******************************
Emem plus aux value={-I(Emem)*V(x)*(Roff-Ron)}
Roff aux minus {Roff}
***********************************************
*Flux computation*
***********************************************
Eflux flux 0 value={SDT(V(plus,minus))}
***********************************************
*Charge computation*
***********************************************
Echarge charge 0 value={SDT(I(Emem))}
***********************************************
* WINDOW FUNCTIONS
* FOR NONLINEAR DRIFT MODELING *
***********************************************
*window function, according to Joglekar
.func f(x,p)={1-(2*x-1)**(2*p)}
*proposed window function
;.func f(x,i,p)={1-(x-sttp(-i))**(2*p)}
.ENDS memristor

How can i get the I-V characteristic in LTspice?
I use dc sweep and it gave me pure linear line
Have you successfully observed the hysteresis loop in LTspice?

 

[fuadfadz]

am i do it wrong?

 

[fuadfadz]

this is what i get when i run dc sweep

 

[BradtheRad]

I know little about memristors but there's animated simulations using them at this link:

Click Yes if a message comes up asking if it can install the java applet.

https://www.falstad.com/circuit/e-mr-sine.html

There are several other simulations of memristor action. It has a whole library of various circuits.

 

[fuadfadz]

thanks for the animated simulations. but still keep bothering me on how to simulate the iv hysteresis on this ltspice.

 

[keith1200rs]

Did you search the forum? There have been quite a few discussions about simulating memristors such as https://www.edaboard.com/threads/202648/

Keith

 

[fuadfadz]

Did you search the forum? There have been quite a few discussions about simulating memristors such as https://www.edaboard.com/threads/202648/

Keith

yes i did. but the problem is, i dont know how to get the hysteresis loop for memristor in LTSpice.

i supposed we have to use dc sweep to get the iv characteristic. but when i used .dc -1.2 1.2 0.1, i get pure linear graph instead of hysteresis loop.

the model did well on PSpice claim by Dalibor and LTSpice by guangyu in https://www.edaboard.com/threads/202648/

btw my transient analysis works well, but not for the iv

 

[keith1200rs]

You need to plot the iv characteristics FROM the transient analysis. You cannot get hysteresis from a single DC sweep. You already have the correct characteristics here: https://www.edaboard.com/threads/253755/#post1086659 you just need to plot current against voltage from that run.

Keith.

 

[fuadfadz]

You need to plot the iv characteristics FROM the transient analysis. You cannot get hysteresis from a single DC sweep. You already have the correct characteristics here: https://www.edaboard.com/threads/253755/#post1086659 you just need to plot current against voltage from that run.

Keith.

thanks for the reply keith. that clarify everything. i did try to plot the characteristic from transient analysis but there is no option to plot the current against voltage. i want to try to work on raw data from the output circuit and plot it on matlab,, is it possible?

 

[keith1200rs]

You can do x-y plots on LTspice. If you have current plotted against time, left click on the x axis (a ruler should be showing for your cursor) then edit the name "time" to whatever you want the x axis to be.

Keith.

 

[fuadfadz]

You can do x-y plots on LTspice. If you have current plotted against time, left click on the x axis (a ruler should be showing for your cursor) then edit the name "time" to whatever you want the x axis to be.

Keith.

SILLY ME! thanks keith! i get my hysteresis loop already! 4 days working on it.

 

[Analogstudent]

Hello all,

Can you please let me know how can I add the memristor symbol to the ltspice so I can add it to my circuit later on?

In other words, how can I add a new element to the previously defined elements in ltspice when I have its behavior as a descriptive code?


Cheers,
Analogstudent

 

[fuadfadz]

anyone know how to test proposed window function by biolek in ltspice?

*proposed window function
.func f(x,i,p)={1-(x-sttp(-i))**(2*p)}

when i try to simulate the circuit if show me an error,, syntax error f():No such function

- - - Updated - - -

anyone know how to test proposed window function by biolek in ltspice?

*proposed window function
.func f(x,i,p)={1-(x-sttp(-i))**(2*p)}

when i try to simulate the circuit if show me an error,, syntax error f():No such function

 

[BradtheRad]

anyone know how to test proposed window function by biolek in ltspice?

*proposed window function
.func f(x,i,p)={1-(x-sttp(-i))**(2*p)}

when i try to simulate the circuit if show me an error,, syntax error f():No such function

When this kind of error happens, it may help to break up a long line of code into several lines. It's a way to get the compiler to point out the error for you.

 

[fuadfadz]

When this kind of error happens, it may help to break up a long line of code into several lines. It's a way to get the compiler to point out the error for you.

i've been trying but still failed. LTspice doesnot allow a function with 3 parameter?

- - - Updated - - -

.func f(x,p)={1-(2*x-1)**(2*p)}

joglekar window fuction working fine on LTspice



.func f(x,i,p)={1-(x-stp(-i))**(2*p)}

but not with biolek window function

 

[keith1200rs]

Try contacting Linear Technology - I believe there is a limit of 2 parameters in a .FUNC but it is not mentioned in the documentation. You could try breaking the function down into two parts.

Keith.

 

[patrickho]

i've been trying but still failed. LTspice doesnot allow a function with 3 parameter?

- - - Updated - - -

.func f(x,p)={1-(2*x-1)**(2*p)}

joglekar window fuction working fine on LTspice



.func f(x,i,p)={1-(x-stp(-i))**(2*p)}

but not with biolek window function

To use biolek window function, you should edit this line 'Gx 0 x value={ I(Emem)*uv*Ron/D**2*f(V(x),p)}' to 'Gx 0 x value={ I(Emem)*uv*Ron/D**2*f(V(x),I(Emem),p)}'
Then comment out joglekar window function, and uncomment biolek window function. This should solve your issue.