orcad pspice User Manual

Monte Carlo analysis

The Monte Carlo analysis calculates the circuit response to 
changes in part values by randomly varying all of the 
model parameters for which a tolerance is specified. This 
provides statistical data on the impact of a device 
parameter’s variance.

With Monte Carlo analysis, model parameters are given 
tolerances, and multiple analyses (DC, AC, or transient) 
are run using these tolerances. 

For EXAMPLE.DSN in Figure 74 on page 12-288, you can 
analyze the effects of variances in the values of resistors 
RC1 and RC2 by assigning a model description to these 
resistors that includes a 5% device tolerance on the 
multiplier parameter R. 

Then you can perform a Monte Carlo analysis. First, the 
simulator performs a DC analysis with the nominal R 
multiplier value for RC1 and RC2. Then it performs a set 
number of additional runs with the R multiplier varied 
independently for RC1 and RC2 within a 5% tolerance.

1

Replace RC1 and RC2 with RBREAK parts, setting 
property values to match the resistors that are being 
replaced (VALUE=10k) and reference designators to 
match previous names.

2

Select PSpice Model from the Edit menu. Create the 
model CRES as follows:

.MODEL CRES RES( R=1 DEV=5% TC1=0.02
+ TC2=0.0045 )

From the File menu, choose Save. By default, Capture 
saves the definition to the model library 
EXAMPLE.LIB and automatically configures the file 
for local use with the current schematic.

3

In Capture, set up a new Monte Carlo analysis as 
shown in Figure 75. The analysis specification tells 
PSpice to do one nominal run and four Monte Carlo 

Monte Carlo analysis is frequently used to 
predict yields on production runs of a 
circuit.

TC1 is the linear temperature coefficient. 
TC2 is the quadratic temperature 
coefficient.

Pspug.book  Page 289  Wednesday, November 11, 1998  1:14 PM