Modeling using a SPICE file

• Here are some of the scaling factors used in SPICE modeling to specify different values 

• Use the node names to create simple circuits using SPICE modeling. Here is a simple RC circuit, whose resistance and capacitance are 1K Ohm and 1u Farad. The RC circuit is connected to a DC voltage source of 5V. 

*----------------------------------------------------------

* Include device model files 

* No files are included

*----------------------------------------------------------

* Define Parameters 

.param SUPPLY=5.0    * Here SUPPLY is created as a parameter 

.option post         * The option is necessary to run the simulations

*----------------------------------------------------------

* Creating the netlist 

R1 n1 n2 1K 

C1 n2 gnd 1uF 

*-----------------------------------------------------------

* Adding Voltage sources 

V1 n1 gnd PULSE (0 'SUPPLY' 2ms 0ms 0ms 5ms 10ms)

*-----------------------------------------------------------

* Stimulus

.tran 0.1ms 50ms

• To conduct a transient analysis, we can vary the voltage with time. In this example, we vary the voltage over time using an independent voltage source. The stimulus can only be applied when .tran command is used. Here, time is varied with an increment of 0.1ps  and the end time of simulation is 80ps. To execute the simulation and plot the waveform using  WaveView (wv) tool. Use the following script to invoke the tool.

hspice <filename>.sp > <output>.lis

wv <filename.tr0> &

* Include device model files 

.include "model-files.pm" * We are using the 32nm hp file from the UMinn 

*----------------------------------------------------------

* Define Parameters 

.param SUPPLY=1.0    * Here SUPPLY is created as a parameter 

.option post         * The option is necessary to run the simulations

*----------------------------------------------------------

* Creating the netlist 

M1 D G S S nmos l=32n w=32n

*-----------------------------------------------------------

* Adding Voltage sources 

VGS G gnd 'SUPPLY'

VDS D gnd 'SUPPLY'

VSB S gnd 0

• To conduct DC analysis, we can sweep the voltages to extrapolate the performance of circuits. A simple DC analysis is conducted on the following circuit. To extract the drain-to-source current (IDS) vs Voltage (VDS) behavior,  We gradually increase the VDS and sweep gate-to-source voltage (VGS). In this example, the VDS varies from 0 to 1.0V, and the IDS current is extrapolated by sweeping VGS between {0.4, 0.6, 0.8, 1.0}

*-----------------------------------------------------------

* Stimulus

.dc VDS 0 'SUPPLY' 0.05 SWEEP VGS 0 'SUPPLY' 0.2

.plot '-1*i(vds)'  * current is often negative in scale for nmos, so reversing the magnitude

• Subcircuits and macros are used to create reusable circuit modules within SPICE modeling, which allows the creation of large-scale circuits using smaller blocks. A subcircuit contains a more detailed device-level circuit netlist, whereas macros contain larger circuit implementations.  

• To create a subcircuit module, we use the keyword  .SUBCKT  and end the netlist .ENDS  . Here is the script for creating a subcircuit file. 

* Creating a Subcircuit

* Start the description with SUBCKT 

.SUBCKT <name> <Terminals list>

* End the description with ENDS

.ENDS 

• Consider the following subcircuit of an inverter circuit, where we can scale the widths of nmos and pmos devices using scale (S). 

* Creating a Inverter subcircuit

* Include the model libraries 

.include "model-files.pm" * We are using the 32nm hp file from the UMinn 

* Defining the Parameters used in the SUBCKT

.param S = 1 

* Start the description with SUBCKT 

.SUBCKT INV IN OUT VDD VSS S

* Creating the PULL-UP

M1 OUT IN VDD VDD pmos l=32n w='32n*S' * Note the parameter 'S' is used inside the inverted commas  

* Creating the PULL-DOWN

M2 OUT IN VSS VSS nmos l=32n w='32n*S'

* End the description with ENDS

.ENDS 

• Instantiating the subcircuit to create the inverter instance 

* Include device model files 

.include "subcircuit_files.sp" * We are using the 32nm hp file from the UMinn 

*----------------------------------------------------------

* Define Parameters 

.param SUPPLY=1.0    * Here SUPPLY is created as a parameter 

.param SCALE=1.0 * Here SCALE is the scaling parameter for inverter sizing

.option post         * The option is necessary to run the simulations

*----------------------------------------------------------

* Creating the netlist 

X1 IN OUT DD SS INV S='SCALE'    * Here the parameter is created after the subckt name

CLOAD OUT GND 1f

*-----------------------------------------------------------

* Adding Voltage sources 

VDS DD gnd 'SUPPLY'

VSB SS gnd 0

VIN IN gnd 0

*-----------------------------------------------------------

* Stimulus

.dc VIN 0 'SUPPLY' 0.05