Lecture 8:

SPICE
Simulation
 Outline
 Introduction to SPICE
 DC Analysis
 Transient Analysis
 Subcircuits
 Optimization
 Power Measurement
 Logical Effort Characterization

8: SPICE Simulation CMOS VLSI Design 4th Ed. 2

 Introduction to SPICE
 Simulation Program with Integrated Circuit Emphasis
– 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

8: SPICE Simulation CMOS VLSI Design 4th Ed. 3

 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!

8: SPICE Simulation CMOS VLSI Design 4th Ed. 4

 Example: RC Circuit
* rc.sp
* David_Harris@hmc.edu 2/2/03
* Find the response of RC circuit to rising input R1 = 2K
*------------------------------------------------ +
* Parameters and models
Vin C1 = Vout
*------------------------------------------------ 100fF -
.option post
*------------------------------------------------
* Simulation netlist
*------------------------------------------------
Vin in gnd pwl 0ps 0 100ps 0 150ps 1.0 1ns 1.0
R1 in out 2k
C1 out gnd 100f
*------------------------------------------------
* Stimulus
*------------------------------------------------
.tran 20ps 1ns
.plot v(in) v(out)
.end

8: SPICE Simulation CMOS VLSI Design 4th Ed. 5

 Result (Graphical)

8: SPICE Simulation CMOS VLSI Design 4th Ed. 6

 Sources
 DC Source
Vdd vdd gnd 2.5
 Piecewise Linear Source
Vin in gnd pwl 0ps 0 100ps 0 150ps 1.0 1ns 1.0
 Pulsed Source
Vck clk gnd PULSE 0 1.0 0ps 100ps 100ps 300ps 800ps

PULSE v1 v2 td tr tf pw per
td tr pw tf
v2

v1 per

8: SPICE Simulation CMOS VLSI Design 4th Ed. 7

 SPICE Elements
Letter Element
R Resistor
C Capacitor
L Inductor
K Mutual Inductor
V Independent voltage source
I Independent current source
M MOSFET
D Diode
Q Bipolar transistor
W Lossy transmission line
X Subcircuit
E Voltage-controlled voltage source
G Voltage-controlled current source
H Current-controlled voltage source
F Current-controlled current source

8: SPICE Simulation CMOS VLSI Design 4th Ed. 8

 Units
Letter Unit Magnitude
a atto 10-18
f fempto 10-15
p pico 10-12
n nano 10-9
u micro 10-6
m milli 10-3
k kilo 103
x mega 106
g giga 109

Ex: 100 femptofarad capacitor = 100fF, 100f, 100e-15

8: SPICE Simulation CMOS VLSI Design 4th Ed. 9
 DC Analysis
* mosiv.sp
*------------------------------------------------
* Parameters and models Ids
*------------------------------------------------
.include '../models/ibm065/models.sp'
.temp 70
.option post 4/2
*------------------------------------------------ Vgs V ds
* Simulation netlist
*------------------------------------------------
*nmos
Vgs g gnd 0
Vds d gnd 0
M1 d g gnd gnd NMOS W=100n L=50n
*------------------------------------------------
* Stimulus
*------------------------------------------------
.dc Vds 0 1.0 0.05 SWEEP Vgs 0 1.0 0.2
.end

8: SPICE Simulation CMOS VLSI Design 4th Ed. 10

 I-V Characteristics
 nMOS I-V
– Vgs dependence
– Saturation

8: SPICE Simulation CMOS VLSI Design 4th Ed. 11

 MOSFET Elements
M element for MOSFET

Mname drain gate source body type

+ W=<width> L=<length>
+ AS=<area source> AD = <area drain>
+ PS=<perimeter source> PD=<perimeter drain>

8: SPICE Simulation CMOS VLSI Design 4th Ed. 12

 Transient Analysis
* inv.sp
* Parameters and models
*------------------------------------------------ 8/2
.param SUPPLY=1.0
.option scale=25n a
.include '../models/ibm065/models.sp' y
.temp 70
.option post 4/2
* Simulation netlist
*------------------------------------------------
Vdd vdd gnd 'SUPPLY'
Vin a gnd PULSE 0 'SUPPLY' 50ps 0ps 0ps 100ps 200ps
M1 y a gnd gnd NMOS W=4 L=2
+ AS=20 PS=18 AD=20 PD=18
M2 y a vdd vdd PMOS W=8 L=2
+ AS=40 PS=26 AD=40 PD=26
* Stimulus
*------------------------------------------------
.tran 0.1ps 80ps
.end

8: SPICE Simulation CMOS VLSI Design 4th Ed. 13

 Transient Results
 Unloaded inverter
– Overshoot
– Very fast
edges

8: SPICE Simulation CMOS VLSI Design 4th Ed. 14

 Subcircuits
 Declare common elements as subcircuits
.subckt inv a y N=4 P=8
M1 y a gnd gnd NMOS W='N' L=2
+ AS='N*5' PS='2*N+10' AD='N*5' PD='2*N+10'
M2 y a vdd vdd PMOS W='P' L=2
+ AS='P*5' PS='2*P+10' AD='P*5' PD='2*P+10'
.ends
 Ex: Fanout-of-4 Inverter Delay
Device
– Reuse inv Under Load on
Shape input Test Load Load
– Shaping 2 8 32 128 512
a b c d e f
X1 X2 X3 X4 X5
– Loading 1 4 16 64 256

8: SPICE Simulation CMOS VLSI Design 4th Ed. 15

 FO4 Inverter Delay
* fo4.sp
* Parameters and models
*----------------------------------------------------------------------
.param SUPPLY=1.0
.param H=4
.option scale=25n
.include '../models/ibm065/models.sp'
.temp 70
.option post
* Subcircuits
*----------------------------------------------------------------------
.global vdd gnd
.include '../lib/inv.sp'
* Simulation netlist
*----------------------------------------------------------------------
Vdd vdd gnd 'SUPPLY'
Vin a gnd PULSE 0 'SUPPLY' 0ps 20ps 20ps 120ps 280ps
X1 a b inv * shape input waveform
X2 b c inv M='H' * reshape input waveform

8: SPICE Simulation CMOS VLSI Design 4th Ed. 16

FO4 Inverter Delay Cont.
X3 c d inv M='H**2' * device under test
X4 d e inv M='H**3' * load
x5 e f inv M='H**4' * load on load
* Stimulus
*----------------------------------------------------------------------
.tran 0.1ps 280ps
.measure tpdr * rising prop delay
+ TRIG v(c) VAL='SUPPLY/2' FALL=1
+ TARG v(d) VAL='SUPPLY/2' RISE=1
.measure tpdf * falling prop delay
+ TRIG v(c) VAL='SUPPLY/2' RISE=1
+ TARG v(d) VAL='SUPPLY/2' FALL=1
.measure tpd param='(tpdr+tpdf)/2' * average prop delay
.measure trise * rise time
+ TRIG v(d) VAL='0.2*SUPPLY' RISE=1
+ TARG v(d) VAL='0.8*SUPPLY' RISE=1
.measure tfall * fall time
+ TRIG v(d) VAL='0.8*SUPPLY' FALL=1
+ TARG v(d) VAL='0.2*SUPPLY' FALL=1
.end

8: SPICE Simulation CMOS VLSI Design 4th Ed. 17

 FO4 Results

8: SPICE Simulation CMOS VLSI Design 4th Ed. 18

 Optimization
 HSPICE can automatically adjust parameters
– Seek value that optimizes some measurement
 Example: Best P/N ratio
– We’ve assumed 2:1 gives equal rise/fall delays
– But we see rise is actually slower than fall
– What P/N ratio gives equal delays?
 Strategies
– (1) run a bunch of sims with different P size
– (2) let HSPICE optimizer do it for us

8: SPICE Simulation CMOS VLSI Design 4th Ed. 19

 P/N Optimization
* fo4opt.sp
* Parameters and models
*----------------------------------------------------------------------
.param SUPPLY=1.0
.option scale=25n
.include '../models/ibm065/models.sp'
.temp 70
.option post
* Subcircuits
*----------------------------------------------------------------------
.global vdd gnd
.include '../lib/inv.sp'
* Simulation netlist
*----------------------------------------------------------------------
Vdd vdd gnd 'SUPPLY'
Vin a gnd PULSE 0 'SUPPLY' 0ps 20ps 20ps 120ps 280ps
X1 a b inv P='P1' * shape input waveform
X2 b c inv P='P1' M=4 * reshape input
X3 c d inv P='P1' M=16 * device under test

8: SPICE Simulation CMOS VLSI Design 4th Ed. 20

 P/N Optimization
X4 d e inv P='P1' M=64 * load
X5 e f inv P='P1' M=256 * load on load
* Optimization setup
*----------------------------------------------------------------------
.param P1=optrange(8,4,16) * search from 4 to 16, guess 8
.model optmod opt itropt=30 * maximum of 30 iterations
.measure bestratio param='P1/4' * compute best P/N ratio
* Stimulus
*----------------------------------------------------------------------
.tran 0.1ps 280ps SWEEP OPTIMIZE=optrange RESULTS=diff MODEL=optmod
.measure tpdr * rising propagation delay
+ TRIG v(c)VAL='SUPPLY/2' FALL=1
+ TARG v(d) VAL='SUPPLY/2' RISE=1
.measure tpdf * falling propagation delay
+ TRIG v(c) VAL='SUPPLY/2' RISE=1
+ TARG v(d) VAL='SUPPLY/2' FALL=1
.measure tpd param='(tpdr+tpdf)/2' goal=0 * average prop delay
.measure diff param='tpdr-tpdf' goal = 0 * diff between delays
.end

8: SPICE Simulation CMOS VLSI Design 4th Ed. 21

 P/N Results
 P/N ratio for equal delay is 2.9:1
– tpd = tpdr = tpdf = 17.9 ps (slower than 2:1 ratio)
– Big pMOS transistors waste power too
– Seldom design for exactly equal delays
 What ratio gives lowest average delay?
.tran 1ps 1000ps SWEEP OPTIMIZE=optrange RESULTS=tpd MODEL=optmod

– P/N ratio of 1.8:1

– tpdr = 18.8 ps, tpdf = 15.2 ps, tpd = 17.0 ps
 P/N ratios of 1.5:1 – 2.2:1 gives tpd < 17.2 ps

8: SPICE Simulation CMOS VLSI Design 4th Ed. 22

 Power Measurement
 HSPICE can measure power
– Instantaneous P(t)
– Or average P over some interval

.print P(vdd)
.measure pwr AVG P(vdd) FROM=0ns TO=10ns

 Power in single gate

– Connect to separate VDD supply
– Be careful about input power

8: SPICE Simulation CMOS VLSI Design 4th Ed. 23

 Logical Effort
 Logical effort can be measured from simulation
– As with FO4 inverter, shape input, load output

Device
Under Load on
Shape input Test Load Load

a
b
X1 c
X2 d
X3 e
M=1 X4
M=h X5 f
M=h2
M=h3
M=h4

8: SPICE Simulation CMOS VLSI Design 4th Ed. 24

 Logical Effort Plots
 Plot tpd vs. h
– Normalize by 
– y-intercept is parasitic delay
– Slope is logical effort
 Delay fits straight line
very well in any process
as long as input slope is
consistent

8: SPICE Simulation CMOS VLSI Design 4th Ed. 25

 Logical Effort Data
 For NAND gates in IBM 65 nm process:

 Notes:
– Parasitic delay is greater for outer input
– Average logical effort is better than estimated

8: SPICE Simulation CMOS VLSI Design 4th Ed. 26

 Comparison

8: SPICE Simulation CMOS VLSI Design 4th Ed. 27