Hello, In this post, we will have a look at the following:

- Setting up 180nm/100nm MOSFET Models in Multisim
- Setting up a memristor model in NI MULTISIM
- A CMOS-Memristor hybrid circuit for edge detection
- Using MATLAB for image analysis

NI Multisim is an excellent tool for simulation of both analog and digital circuits. One reason I like it over LTSpice or PSpice is the ease with which one can simulate mixed-signal circuitry. Using Multisim along with MATLAB allows conversion of image(pixel by pixel) to its a corresponding discrete voltage signal and vice versa.

We can import PSPICE models to multisim using its component wizard. I’ll elaborate it further:

# Setting up 180nm/100nm MOSFET Models in Multisim

Following is the code for NMOS and PMOS using 180nm fabrication technology:

Source: https://user.eng.umd.edu/~newcomb/courses/spring2010/303/tsmc180nmcmos.lib

.MODEL TSMC180nmN NMOS ( LEVEL = 7 +VERSION = 3.1 TNOM = 27 TOX = 4.1E-9 +XJ = 1E-7 NCH = 2.3549E17 VTH0 = 0.354505 +K1 = 0.5733393 K2 = 3.177172E-3 K3 = 27.3563303 +K3B = -10 W0 = 2.341477E-5 NLX = 1.906617E-7 +DVT0W = 0 DVT1W = 0 DVT2W = 0 +DVT0 = 1.6751718 DVT1 = 0.4282625 DVT2 = 0.036004 +U0 = 327.3736992 UA = -4.52726E-11 UB = 4.46532E-19 +UC = -4.74051E-11 VSAT = 8.785346E4 A0 = 1.6897405 +AGS = 0.2908676 B0 = -8.224961E-9 B1 = -1E-7 +KETA = 0.021238 A1 = 8.00349E-4 A2 = 1 +RDSW = 105 PRWG = 0.5 PRWB = -0.2 +WR = 1 WINT = 0 LINT = 1.351737E-8 *+XL = -2E-8 XW = -1E-8 + DWG = 1.610448E-9 +DWB = -5.108595E-9 VOFF = -0.0652968 NFACTOR = 2.4901845 +CIT = 0 CDSC = 2.4E-4 CDSCD = 0 +CDSCB = 0 ETA0 = 0.0231564 ETAB = -0.058499 +DSUB = 0.9467118 PCLM = 0.8512348 PDIBLC1 = 0.0929526 +PDIBLC2 = 0.01 PDIBLCB = -0.1 DROUT = 0.5224026 +PSCBE1 = 7.979323E10 PSCBE2 = 1.522921E-9 PVAG = 0.01 +DELTA = 0.01 RSH = 6.8 MOBMOD = 1 +PRT = 0 UTE = -1.5 KT1 = -0.11 +KT1L = 0 KT2 = 0.022 UA1 = 4.31E-9 +UB1 = -7.61E-18 UC1 = -5.6E-11 AT = 3.3E4 +WL = 0 WLN = 1 WW = 0 +WWN = 1 WWL = 0 LL = 0 +LLN = 1 LW = 0 LWN = 1 +LWL = 0 CAPMOD = 2 XPART = 0.5 +CGDO = 7.7E-10 CGSO = 7.7E-10 CGBO = 1E-12 +CJ = 1.010083E-3 PB = 0.7344298 MJ = 0.3565066 +CJSW = 2.441707E-10 PBSW = 0.8005503 MJSW = 0.1327842 +CJSWG = 3.3E-10 PBSWG = 0.8005503 MJSWG = 0.1327842 +CF = 0 PVTH0 = 1.307195E-3 PRDSW = -5 +PK2 = -1.022757E-3 WKETA = -4.466285E-4 LKETA = -9.715157E-3 +PU0 = 12.2704847 PUA = 4.421816E-11 PUB = 0 +PVSAT = 1.707461E3 PETA0 = 1E-4 PKETA = 2.348777E-3 )

.MODEL TSMC180nmP PMOS ( LEVEL = 7 +VERSION = 3.1 TNOM = 27 TOX = 4.1E-9 +XJ = 1E-7 NCH = 4.1589E17 VTH0 = -0.4120614 +K1 = 0.5590154 K2 = 0.0353896 K3 = 0 +K3B = 7.3774572 W0 = 1E-6 NLX = 1.103367E-7 +DVT0W = 0 DVT1W = 0 DVT2W = 0 +DVT0 = 0.4301522 DVT1 = 0.2156888 DVT2 = 0.1 +U0 = 128.7704538 UA = 1.908676E-9 UB = 1.686179E-21 +UC = -9.31329E-11 VSAT = 1.658944E5 A0 = 1.6076505 +AGS = 0.3740519 B0 = 1.711294E-6 B1 = 4.946873E-6 +KETA = 0.0210951 A1 = 0.0244939 A2 = 1 +RDSW = 127.0442882 PRWG = 0.5 PRWB = -0.5 +WR = 1 WINT = 5.428484E-10 LINT = 2.468805E-8 *+XL = -2E-8 XW = -1E-8 +DWG = -2.453074E-8 +DWB = 6.408778E-9 VOFF = -0.0974174 NFACTOR = 1.9740447 +CIT = 0 CDSC = 2.4E-4 CDSCD = 0 +CDSCB = 0 ETA0 = 0.1847491 ETAB = -0.2531172 +DSUB = 1.5 PCLM = 4.8842961 PDIBLC1 = 0.0156227 +PDIBLC2 = 0.1 PDIBLCB = -1E-3 DROUT = 0 +PSCBE1 = 1.733878E9 PSCBE2 = 5.002842E-10 PVAG = 15 +DELTA = 0.01 RSH = 7.7 MOBMOD = 1 +PRT = 0 UTE = -1.5 KT1 = -0.11 +KT1L = 0 KT2 = 0.022 UA1 = 4.31E-9 +UB1 = -7.61E-18 UC1 = -5.6E-11 AT = 3.3E4 +WL = 0 WLN = 1 WW = 0 +WWN = 1 WWL = 0 LL = 0 +LLN = 1 LW = 0 LWN = 1 +LWL = 0 CAPMOD = 2 XPART = 0.5 +CGDO = 7.11E-10 CGSO = 7.11E-10 CGBO = 1E-12 +CJ = 1.179334E-3 PB = 0.8545261 MJ = 0.4117753 +CJSW = 2.215877E-10 PBSW = 0.6162997 MJSW = 0.2678074 +CJSWG = 4.22E-10 PBSWG = 0.6162997 MJSWG = 0.2678074 +CF = 0 PVTH0 = 2.283319E-3 PRDSW = 5.6431992 +PK2 = 2.813503E-3 WKETA = 2.438158E-3 LKETA = -0.0116078 +PU0 = -2.2514581 PUA = -7.62392E-11 PUB = 4.502298E-24 +PVSAT = -50 PETA0 = 1E-4 PKETA = -1.047892E-4 )

for 100nm, the MOSFET SPICE code can be found here.

The above code can be imported using the component wizard.

**Note:- For MULTISIM, change the ‘LEVEL’ parameter in the above codes from 7 to 8.**

# Setting up a memristor model in NI MULTISIM

There are mainly 3 types of memristor models: Linear, Non-Linear, and TEAM. I mostly use a Non-linear model with Prodomakis or Jinxiang window functions. Have a look at my previous post for an overview of all available memristor models and window function.

Below is the Non-linear memristor model with jinxiang window function:

************************************ * Jinxiang non-linear memristor model * * Please acknowledge when used. * Written by :- Udit agarwal ************************************ .param ron = 100 .param roff = 16000 .param d = 40E-9 .param uv = 10E-15 .param p = 7 .param x0 = 0.076 .param j = 1 .param a = 0.9 Gx 0 x value={I(Emem)*uv*ron/d**2*f(V(x),I(Emem),p)} Cx x 0 1 Raux x 0 1000000 Emem plus aux value={-I(Emem)*V(x)*(roff-ron)} roff aux minus {roff} Eflux flux 0 value={SDT(V(plus,minus))} Echarge charge 0 value={SDT(I(Emem))} * window function, according to Jinxiang .func f(x,i,p)=j*{1-pow((a*pow((x - stp(-i)),(2*p)) + (1 - a)),(p))}

The above model can again be imported in Multisim using Component Wizard.

After importing the model, it can be verified using the following circuit:

Change in memristance concerning time can be seen in the adjoining graph, which thus confirms the working of the model.

**Note- While performing transient analysis of the memristor model in Multisim, change the initial condition setting to ‘User-defined’, otherwise simulation might not converge.**

# A CMOS-Memristor hybrid circuit for edge detection

- This circuit is primarily a region segmentation circuit where a memristor can control the intensity of response.
- It can be used for Edge detection, color extraction from an image, etc.

The complete circuit consists of 3 parts. First and the last part makes up the variable threshold NOT gate, which is responsible for setting up lower and upper limits between which whenever the input signal lies, output comes in the form of a spike.

# Using MATLAB for image analysis

Here MATLAB is being used to convert an image sequentially(Pixel by Pixel) to an electrical discrete signal, which is then passed through the circuit. Circuit’s output is then converted using another script to the output image.

Below are the MATLAB scripts:

clc; clear all; img = imread('C:\Users\udit agarwal\Desktop\Memristor\guassian_sun.jpg'); img = imresize(img,[55 55],'bicubic'); % Convert a RGB to WB if(size(img,3) == 3) img = rgb2gray(img); end; img_serial = img(:); size_1 = size(img_serial,1) - 1; img_serial = im2uint16(img_serial); img_serial = [0:1:(size_1) ; img_serial']; img_serial = double(img_serial'); img_serial(:,2) = img_serial(:,2)./max(img_serial(:,2)); img_serial(:,2) = img_serial(:,2).*1.6; img_serial(:,1) = img_serial(:,1)./200;

output can be probed from the img_serial variable.

clc; clear; a = csvread('C:\Users\udit agarwal\Desktop\Memristor\pixel_guassian_mem.csv'); b = []; b = horzcat(b,a(:,1)); b = horzcat(b,a(:,2)); b = horzcat(b,a(:,5)); a = []; for i=1:size(b,1) if(mod(b(i),0.005) == 0) a = vertcat(a,b(i,:)); end; end; out = a(:,2)'; in = a(:,3)'; %Input data dd_inp = []; for j=0:(floor(sqrt(size(a,1))) - 1) dd_inp = vertcat(dd_inp,in(55*j + 1:55*(j+1))); end; dd_inp = dd_inp./max(dd_inp(:)); dd_inp = dd_inp*255; dd_inp = ceil(dd_inp); %output data dd_out = []; for j=0:(floor(sqrt(size(a,1))) - 1) dd_out = vertcat(dd_out,out(55*j + 1:55*(j+1))); end; dd_out = dd_out./max(dd_out(:)); dd_out = dd_out*255; dd_out = ceil(dd_out); subplot(1,2,1); imshow(dd_inp,[0 255]) title('Input image'); subplot(1,2,2); imshow(dd_out,[0 255]) title('Output image');

The output of the analog signal can be stored in a CSV file(line 3), which is then processed to convert it into an image.

It is so nice to read this post. I have set up circuit model, but there are some problems during simulating. What are the parameters of pulse voltage?