Transcript Presentation - aslanistan.com
SPICE USING LTSPICE
DR. ASLAN TEXAS STATE UNIVERSITY
• Introduction to SPICE • DC Analysis • Transient Analysis • AC Analysis • Subcircuits • Optimization • Power Measurement
OUTLINE
INTRODUCTION TO SPICE
•
S
imulation
P
rogram with
I
ntegrated
C
ircuit
E
mphasis
• Developed in 1970’s at Berkeley • Many commercial versions are available • HSPICE is a robust industry standard • Has many enhancements that we will use •
Written in FORTRAN for punch-card machines
• • Circuits elements are called cards Complete description is called a SPICE deck
WRITING SPICE DECKS
•
Writing a SPICE deck is like writing a good program
• Plan: sketch schematic on paper or in editor • Modify existing decks whenever possible • Code: strive for clarity • • Start with name, email, date, purpose Generously comment •
Test:
• • • Predict what results should be Compare with actual
Garbage In, Garbage Out!
SOME FACTS AND RULES ABOUT SPICE
• • • • • • • Spice is not case sensitive. Rsource and RsOuRcE and RSOURCE are equivelent.
All element names must be unique. You can't have two capacitors that both are named “C1”.
The first line in the data file is used as a title. Spice will ignore this line as circuit data. Put your name and title.
There must be a node designated "0" (Zero). This is the reference node against which all voltages are calculated.
Each node must have at least two elements attached to it. The last line in any data file must be ".END" (a period followed by the word "end.") All lines that are not blank (except for the title line) must have a character in column 1, the leftmost position on the line.
• • • • Use "*" (an asterisk) in column 1 in order to create a comment line.
Use "+" (plus sign) in column 1 in order to continue the previous line (for better readability of very long lines).
Use "." (period) in column 1 followed by the rest of the "dot command" to pass special instructions to the program.
Use the designated letter for a part in column 1 followed by the rest of the name for that part (no spaces in the part name).
• • Use "whitespace" (spaces or tabs) to separate data fields on a line.
Use ";" (semicolon) to terminate data on a line if you wish to add commentary information on that same line.
SPICE ELEMENTS
k x g p n u m Letter f a
UNITS
Unit atto fempto pico nano micro mili kilo mega giga Magnitude 10 -18 10 -15 10 -12 10 -9 10 -6 10 -3 10 3 10 6 10 9 Ex: 100 femptofarad capacitor = 100fF, 100f, 100e-15
SOURCES - DC
; "V" after "16.0" is optional 24m ; "QE" is +node & "qc" is -node ; "dc" not really needed -1.8E4 ; same as above 0V ; V-source used as ammeter
SOURCES - AC
• DC Source Vname Iname n+ n+ n n Type Type Value Value Phase (Deg) Phase (Deg) Vac 4 1 Vba 2 5 Ix 3 6 Isv 12 9 AC 120V AC 240 30 AC 10.0A -45 AC 25mA ; phase angle 0 degrees ; phase angle -45 degrees ; 25 milliamps @ 0 degrees
SOURCES – DEPENDENT
• Voltage controlled voltage source: Ename n+ n nc+ nc Voltage Gain Value Ebar efix 17 8 42 18 24.0; gain is 24 3 1 0 11 -20.0; same as above Ellen 12 0 20 41 16.0
• Voltage controlled current source: Gname Glab 23 17 G1 12 9 Grad 19 40 Grad 19 40 Grad 40 19 n+ n nc+ nc 1 8 6 99 99 0 3 2.5
4E-2 99 0.65
6 -0.65 ; same as above 6 0.65 ; etc.
Value
SOURCES – DEPENDENT (CONT.)
• Current controlled voltage source: Hname N1 N2 Hvx 20 12 Vhx Vhx 80 76 DC Hab 10 0 V20 V20 15 5 DC HAL 20 99 Vuse Vuse 3 5 DC Vcontrol Value 50.0
0V ; controls Hvx 75.0
0V ; controls Hab 10.0
20V ; actual voltage source • Current controlled current source: Fname N1 N2 Ftrn 81 19 Vctl Vclt 23 12 DC Fcur 63 48 Vx Vx 33 71 DC F3 V1 2 0 V1 3 1 DC Vcontrol Value 50.0
0V ; controls Ftrn 20.0
0V ; controls Fcur 15.0
0V ; controls F3
SOURCES – PULSE
Vname n+ n- Pulse(V1 V2 Td Tr Tf Tw Period) V1 V2 Td Tr Tf Tw Period : Initial voltage : Peak voltage : Initial delay time : Rise time; : Fall time; : Pulse width : Period. Vs 1 0 Pulse(0V 10V 0 0.1 0.1 0.9 2) Vs 1 0 Pulse(0V 10V 0s 100ms 100ms 900ms 2s) Vs 1 0 Pulse(0 10 0 100m 100m 900m 2)
SOURCES –
SINUSOIDAL
Vname n+ n- Sin(Vo Va fr Td Theta phase) Vname = Vo + Va e [-Theta.(t - Td)] sin[2pi.fr (t - Td) + (Phase/360)] Vo : Offset voltage in volt.
Va : Amplitude in volt.
fr : The frequency in Hz.
Td : Delay in seconds Theta : Damping factor per second Phase : Phase in degrees Vs 1 0 SIN(2V 5V 2Hz 200ms 2Hz 30d) VG 1 2 SIN(5 10 50 0.2 0.1) VG2 3 4 SIN(0 10 50)
SOURCES – PIECEWISE LINEAR SOURCE
Vname n+ n- PWL(T1 V1 T2 V2 T3 V3 ...) T1 : Time for the first point V1 : Voltage for the first point T2 : Time for the second point V2 : Voltage for the second point Vgpwl 1 2 PWL(0 0 10U 5 100U 5 110U 0)
CIRCUIT ANALYSIS - .OP
• .OP (Operating Point Analysis) Example_OP.CIR
Vs 1 0 DC 20.0V ; note the node placements Ra 1 2 5.0k
Rb 2 0 4.0k
Rc 3 0 1.0k
Is 3 2 DC 2.0mA ; note the node placements .OP
.END
If you need some values use .PRINT DC V(3,2) I(Ra)
CIRCUIT ANALYSIS - .TRAN
• * .TRANTransient Analysis prt_stp t_max prt_dly max_stp .TRAN 20us 20ms 8ms 10us UIC 1. The following example performs and prints the transient analysis every 1 ns for 100 ns.
.TRAN 1NS 100NS 2. The following example performs the calculation every 10 ns for 1 µs; the initial DC operating point calculation is bypassed, and the nodal voltages specified in the .IC statement (or by IC parameters in element statements) are used to calculate initial conditions. .TRAN 10NS 1US UIC
CIRCUIT ANALYSIS - .TRAN
Example_TRAN.cir
Rp 0 1 1.0
Lp 1 0 8mH IC=20A Cp 1 0 10mF IC=0V .TRAN 500us 100ms 0s 500us UIC .PROBE
.END
DATA TRANSFER TO MATLAB
Assume I have the previous circuit Example_TRAN.cir. After you run Simulate now you can import your data to MATLAB for further analysis. In LTSpice go to File → Export Change the file name. Keep the extension (mace it .xls if you want to open in excel) Highlight the data values (Transient analysis time will be added) Now you can open your MATLAB and relocate MATLAB directory where you saved “Example_ TRAN.txt” file.
DATA TRANSFER TO MATLAB (CONT.)
Now you can open your MATLAB and relocate MATLAB directory where you saved “Example_ TRAN.txt” file. In MATLAB command window type >> load Example_TRAN.txt
Txt file will create and error. This is due to forst line of the txt file.
xls file MATLAB cannot read that first line as data. Delete that line and save your file. Do not forget the order of the columns. (1 st Column is time, 2 nd I(Cp) and 3 rd one is I(Lp)) >> load Example_TRAN.txt
In workspace of MATLAB you will see the loaded data. It hae 202 rows and 3 columns. Next step we will save the data as time, I(Cp) and I(Lp).
DATA TRANSFER TO MATLAB (CONT.)
In workspace of MATLAB you will see the loaded data. It hae 202 rows and 3 columns. Next step we will save the data as time, I(Cp) and I(Lp). >> t=Example_TRAN(:,1); %This will save t as time variable >> I_Cp=Example_TRAN(:,2); %This will save I_Cp as time I(Cp) >> I_Lp=Example_TRAN(:,3); %This will save I_Lp as time I(Lp) Your work place shoul look like this Now we can plot these >> >> plot (t, I_Cp, t,I_Lp)
CIRCUIT ANALYSIS - .AC
* type .AC LIN .AC LIN .AC DEC #points start 1 60Hz 11 20 100 1Hz stop 60Hz; <== what we want now.
200; <== a linear range sweep 10kHz; <== a logarithmic range sweep .PRINT AC VM(30,9) VP(30,9); magnitude & angle of voltage .PRINT AC IR(Rx) II(Rx); real & imag. parts Rx current .PRINT AC VM(17) VP(17) VR(17) VI(17); the whole works on node 17
CIRCUIT ANALYSIS - .AC
Example_AC.cir
Vs 1 0 AC 120V 0 Rg 1 2 0.5
Lg 2 3 3.183mH
Rm 3 4 16.0
Lm 4 0 31.83mH
Cx 3 0 132.8uF
.AC LIN 1 60 60 .PRINT AC VM(3) VP(3) IM(Rm) IP(Rm) IM(Cx) IP(Cx) .END
CIRCUIT ANALYSIS - .AC
First-order low-pass RC filter Vin 1 0 AC 1.0V
Rf 1 2 1.59
Cf 2 0 100uF .AC DEC 20 100Hz 100kHz .PROBE
.END
Second-Order High-Pass Filter Vin 1 0 AC 10V Rf 1 2 4.0
CF 2 3 2.0uF
Lf 3 0 127uH .AC DEC 20 100Hz 1MEG .PROBE
.END
* .SUBCKT Example_1 5 12 18 Iw 10 12 DC 10A Ra name 5 12 5.0
nodelist Rb Rc 12 13 2.0
Rd .ENDS
5 13 4.0
5 18 8.0
Re 13 18 3.0
Rf 10 13 1.0
Rg 10 18 6.0
SUBCIRCUITS
Subcircuit Example No. 1 * Ra Rb Rd .ENDS
Vs 1 name 5 12 2.0
5 13 5.0
Rc 12 13 2.0
5 18 8.0
Re 13 18 3.0
Rf 10 13 1.0
Rg 10 18 6.0
nodelist .SUBCKT Example_1 5 12 18 Iw 10 12 DC 10A 0 DC 50V Ra 1 2 1.0 ; different from Ra above Rb Rc Rd 7 3 6 4 3.0 ; different from Rb above 0 25.0 ; different from Rc above 0 45.0 ; different from Rd above * X1 X2 .END
nodelist 2 7 4 6 name 3 Example_1 5 Example_1
.SUBCKT OpAmp p_in n_in com out Ex int com p_in n_in 1e5 Ri p_in n_in 500k Ro int out 50.0
.ENDS
SUBCIRCUITS
Subcircuit Example No. 2 - Inverting OpAmp .SUBCKT OpAmp p_in n_in com out Ex int com p_in n_in 1e5 Ri p_in n_in 500k Ro int out 50.0
.ENDS
Vg 1 0 DC 50mV Rg 1 Rf 2 3 2 5k 50k RL 3 X1 0 .END
0 2 20k 0 3 OpAmp
CIRCUIT ANALYSIS
Voltage Divider Circuit VCC 4 0 R1 R2 4 1 1 0 DC 10K RMOD 1 .MODEL RMOD RES(R=1) .STEP RES RMOD(R) .1k, 15k, 1k RC 4 3 2.7K
12V RE 2 0 1K Q1 3 .model Q2N3904 1 2 Q2N3904 Model for 2N3904 NPN BJT (from Eval library in Pspice) NPN(Is=6.734f Xti=3 Eg=1.11 Vaf=74.03 Bf=416.4 Ne=1.259
+ + + Ise=6.734f Ikf=66.78m Xtb=1.5 Br=.7371 Nc=2 Isc=0 Ikr=0 Rc=1 Cjc=3.638p Mjc=.3085 Vjc=.75 Fc=.5 Cje=4.493p Mje=.2593 Vje=.75
Tr=239.5n Tf=301.2p Itf=.4 Vtf=4 Xtf=2 Rb=10) .OP
.PRINT DC I(VCC) I(RC) .END
CIRCUIT ANALYSIS
Voltage Divider Circuit VCC 4 R1 4 1 0 10K R2 1 0 RMOD 1 .MODEL RMOD RES(R=1) .STEP RES RMOD(R) .1k, 15k, 1k RC 4 3 2.7K
DC RE Q1 2 3 .include bjt.lib
.OP
.PRINT DC I(VCC) I(RC) .END
0 1 1K 2 12V Q2N3904
THEVENIN’S THEOREM
Thevenin Example No. 1 Vs 2 5 DC 100V Vc 2 3 DC 0V; controls Fx Fx 6 7 Vc 4.0; gain = 4 * n+ n- NC+ NC gain Ex 2 1 5 4 3.0; gain = 3 R1 3 4 5.0
R2 4 7 5.0
R3 5 4 4.0
R4 7 0 4.8
R5 5 6 1.0
R10 1 0 1MEG; satisfies PSpice * out_var input_source .TF V(1,0) Vs .END
REFERENCES
• http://www.uta.edu/ee/hw/pspice/ • http://cmosedu.com/ • http://www.seas.upenn.edu/~jan/spice/spice.overview.html#Output