Issue link: https://resources.pcb.cadence.com/i/1180526
PSpice User Guide Monte Carlo and sensitivity (worst-case) analyses October 2019 567 Product Version 17.4-2019 © 1999-2019 All Rights Reserved. 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. Monte Carlo analysis is frequently used to predict yields on production runs of a circuit. With Monte Carlo analysis, model parameters are given tolerances, and multiple analyses (DC, AC, or transient) are run using these tolerances. For EXAMPLE.OPJ in Figure 13-1 on page 566, 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. The steps for adding the 5% device tolerance are given below. 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. To modify example.opj and set up simulation 1. Replace RC1 and RC2 with RBREAK parts from the BREAKOUT.OLB part library, setting property values to match the resistors that are being replaced (VALUE=10k) and reference designators to match previous names. 2. Select an RBREAK part and choose PSpice Model from the Edit menu. The Model Editor window appears. 3. Create the model CRES by replacing the model text: .model Rbreak RES R=1 with the text: .MODEL CRES RES( R=1 DEV=5% TC1=0.02 + TC2=0.0045 ) Where TC1 is the linear temperature coefficient. TC2 is the quadratic temperature coefficient.