Engineering 77 Lab 2: Spicey

Engineering 77 Lab 2: Spicey

Aron Dobos, Tyler Strombom

19 September 2005

Abstract

In this lab SPICE netlists and MATLAB programs were written to simulate a variety of non-linear diode circuits. The Matlab approach involved performing a modified nodal analysis and using the Newton-Raphsen method for iteratively solving the non-linear equations. The netlists, code, and results for the various tasks are documented below.

Task 1

The goal of task 1 was to plot the voltages at nodes 1, 2, and 3 for the circuit below using SPICE and a Matlab program using the modified nodal analysis technique that we learned in class.

Figure 1. Circuit for Task 1

The following is the SPICE deck and Matlab program followed by the graphs of the voltages at nodes 1, 2, and 3.

SPICE Netlist for Task 1

*Control section determines type of analysis

.control

destroy all

echo

TRAN 0.01 2

plot V(1) V(2) V(3)

.endc

*These next lines give circuit layout (netlist)

R1 1 2 1k

R2 2 3 4k

R3 3 0 1k

*form of sinusoid -- SIN(VO VA FREQ TD THETA)

VVin 1 0 SIN(0 4 1 0 0)

.end

Matlab Code for Task 1

% Set Circuit Values

R1=1000;

R2=4000;

R3=1000;

DT = 1E-6; %Time Increment

t=0:DT:0.002; %Time Vector

Vin=4*sin(2*pi*1000*t);

% Allocate memory for arrays

V1=zeros(size(t)); V2=zeros(size(t)); V3=zeros(size(t));

% Initial Conditions

V1(1)=0; V2(1)=0; V3(1)=0;

A=[1/R1 -1/R2 0 1;

-1/R1 1/R1+1/R2 -1/R2 0;

0 -1/R2 1/R2+1/R3 0;

1 0 0 0];

invA=inv(A);

for i=2:length(t),

b=[0 0 0 Vin(i)]';

x=invA*b;

V1(i)=x(1);

V2(i)=x(2);

V3(i)=x(3);

end

plot(t*1000, V1, 'r',t*1000,V2,'g',t*1000,V3,'b');

axis([0 2 -4 4]);

grid on

title('Task 1');

xlabel('Time (mS)');

Figure 2. Plot of Voltages at Nodes 1, 2, and 3 using SPICE

Figure 3. Plot of Voltages at nodes 1, 2, and 3 using MATLAB

Task 2

The goal of task 2 was to plot the voltages at nodes 1, 2, and 3 for the circuit below using SPICE and a Matlab program using the modified nodal analysis technique that we learned in class.

Figure 4. Circuit for Task 2

The following is the SPICE deck and Matlab program followed by the graphs of the voltages at nodes 1, 2, and 3.

SPICE NetList for Task 2

*Control section determines type of analysis

.control

destroy all

echo

TRAN 0.01MS 2MS

plot V(1) V(2) V(3)

.endc

*These next lines give circuit layout (netlist)

R1 1 2 1k

R2 2 3 1k

R3 3 0 1k

C1 2 3 1u

*form of pulse -- PULSE(V1 V2 TD TR TF PW PER)

VVin 1 0 PULSE(0 5 0 0 0 .5m 1m)

.end

Matlab Code for Part 2

% Task 2

% Set Circuit Values

R1=1000;

R2=1000;

R3=1000;

C1=1E-6;

DT=1E-6; %Time increment

t=0:DT:0.002; %Time vector

Vin=5*(1+square(t*1000*2*pi))/2; %5V, 1kHz square wave for Vin.

% Allocate memory for arrays.

V1=zeros(size(t)); V2=zeros(size(t)); V3=zeros(size(t));

%Initial conditions

V1(1)=0; V2(1)=0; V3(1)=0;

Rc = DT/C1;

A = [-1/R1 1/R1 0 1;

1/R1 (-1/R1-1/R2-1/Rc) (1/R2+1/Rc) 0;

0 (1/Rc+1/R2) (-1/Rc-1/R2-1/R3) 0;

1 0 0 0 ]

invA=inv(A);

for i=2:length(t),

Vc_t0=V2(i-1)-V3(i-1);

IC = Vc_t0*C1/DT;

b = [0 -IC IC Vin(i)]';

x=invA*b;

V1(i) = x(1);

V2(i) = x(2);

V3(i) = x(3);

end

plot(t*1000,V1,'r',t*1000,V2,'g',t*1000,V3,'b');

axis([0 2 -5 5]);

grid on

title('E77 Lab 2 Part 2');

xlabel('Time (mS)');

ylabel('Voltage (V)');

legend('V1', 'V2', 'V3');

Figure 5. Plot of Voltages at Nodes 1, 2, and 3 using SPICE

Figure 6. Plot of Voltages at Nodes 1, 2, and 3 using MATLAB

Task 3

The goal of task 3 was to plot the voltages at nodes 1, 2, and 3 for the circuit below using SPICE and a Matlab program using the modified nodal analysis technique that we learned in class.

Figure 7. Circuit for Task 3

The following is the SPICE deck and Matlab program followed by the graphs of the voltages at nodes 1, 2, and 3.

SPICE NetList for Task 3

*Control section determines type of analysis

.control

destroy all

echo

TRAN 0.01MS 2MS

plot V(1) V(2) V(3)

.endc

*These next lines give circuit layout (netlist)

R1 1 2 1k

R2 2 3 4k

R3 3 0 1k

D1 2 1 DMOD

D2 2 3 DMOD

*form of sinusoid -- SIN(VO VA FREQ TD THETA)

VVin 1 0 SIN(0 4 1000 0 0)

.MODEL DMOD D Is=1.0E-15 n=1

.end

Matlab Code for Part 3

% Task 3

R1=1000;

R2=4000;

R3=1000;

Is=1E-15;

VT=25e-3;

DT=1E-6;

t=0:DT:0.002;

V3=4*sin(2*pi*1000*t);

%Allocate Memory for Arrays

V2=zeros(size(t));

V1=zeros(size(t));

iter=0;

err=1; %Initialize error to something large to start loop

V0=[0.5 0.5]'; %Initial guess for node voltage

for i=1:length(V2),

while err>0.0001,

iter=iter+1; %Count iterations

e1=exp((V0(1)-V3(i))/VT);

e2=exp((V0(1)-V0(2))/VT);

fv1=(V0(1)-V3(i))/R1+(V0(1)-V0(2))/R2+Is*(e1-1)+Is*(e2-1);

fv2=(V0(2)-V0(1))/R2+V0(2)/R3-Is*(e2-1);

dfv1dv1=1/R1+1/R2+Is*e1/VT+Is*e2/VT;

dfv1dv2=-1/R1-Is*e2/VT;

dfv2dv1=-1/R2-Is*e2/VT;

dfv2dv2=1/R2+1/R3+Is*e2/VT;

F=[fv1 fv2]'; %Function we wish to find zero of

J=[dfv1dv1 dfv1dv2; dfv2dv1 dfv2dv2]; %Jacobian

Vnew=V0-inv(J)*F;

err=sum(abs(Vnew-V0)./abs(Vnew+V0)); %error

V0=Vnew; %New guess

end

V2(i)=V0(2);

V1(i)=V0(1);

err=1;

end

iter

plot(t,V1,'g',t,V2,'b',t,V3,'r')

xlabel('Time(ms)');

ylabel('Voltage');

title('Task 3');

grid;

Figure 8. Plot of Voltages at Nodes 1, 2, and 3 using SPICE

Figure 9. Plot of Voltages at Nodes 1, 2, and 3 using MATLAB

Task 4

The goal of task 4 was to plot the voltages at nodes 1, 2, and 3 for the circuit below using SPICE and a matlab program using the modified nodal analysis technique that we learned in class.

Figure 10. Circuit for Task 4

The following is the SPICE deck and Matlab program followed by the graphs of the voltages at nodes 1, 2, and 3.

SPICE NetList for Task 4

*Control section determines type of analysis

.control

destroy all

echo

TRAN 0.01MS 2MS

plot V(1) V(2)

.endc

*These next lines give circuit layout (netlist)

R1 2 0 1k

C1 2 0 1u

D1 1 2 DMOD

*form of sinusoid -- SIN(VO VA FREQ TD THETA)

VVin 1 0 SIN(0 4 1k 0 0)

.MODEL DMOD D Is=1.0E-15 n=1

.end

Matlab Code for Task 4

%% E77 Lab 2 part 4

%% half-wave rectifier circuit, 1uF reservoir, 1k load

clc

DT=1e-6;

t=0:DT:.002;

Is=1e-15;

n=1;

C = 1e-6;

R = 1000;

VT = 0.025;

Vin = 4*sin(2*pi*1000*t);

V2 = zeros(size(t));

Vd = zeros(size(t));

Id = zeros(size(t));

V2(1) = 0; % initial condition on the capacitor

for i=2:length(t),

Ic = C/DT*V2(i-1);

Rc = DT/C;

Vd(i) = part4_newton(Vin(i), R, Ic, Rc, Is, n, -10, 10, Vin(i)-V2(i-1));

Id(i) = Is*(exp(Vd(i)/(n*VT))-1);

Gdiode = Is/(n*VT)*exp(Vd(i)/(n*VT));

V2(i) = (Vin(i)*Gdiode + Id(i) + Ic)/(Gdiode + 1/Rc + 1/R);

end

plot(t*1000,Vin, 'r', t*1000, V2, 'g')

grid

title('E77 Lab 2 Part 4: Half-wave rectifier, 4Vp-p, 1uF reservoir, 1k load');

xlabel('Time (ms)');

ylabel('Voltage (V)');

legend('Vin', 'V2');

function [Vd] = part4_newton(VIN, R, IC, RC, IS, N, vmin, vmax, guess)

% newton's method for diode dc op

% example: Vdiode = part4_newton(vin, R, Ic, Rc, Is, n, -2, 2);

threshold = 0.00001; % accuracy of Vd result

max_iter = 50; % maximum number of iterations

Vd = guess; % start with a reasonable guess

VT = 0.025; % thermal voltage

for i=1:max_iter,

f = IS*(exp(Vd/(N*VT))-1) + IC - (VIN-Vd)/RC - (VIN-Vd)/R;

df = IS/(N*VT)*exp(Vd/(N*VT)) +1/RC + 1/R;

dx = f/df;

Vd = Vd - dx; % x1 = x - f(x)/df(x)

if (Vd < vmin || Vd > vmax)

disp('newton: exceeded bounds');

return;

end

% if change from previous Vd value was smaller than

% the accuracy threshold, we're done, so return.

if (abs(dx) < threshold)

return;

end

disp('newton: failed to converge in 50 iterations');

return;

Figure 11. Plot of Voltages at Node 2 using SPICE

Figure 12. Plot of Voltages at Node 2 using MATLAB