Issue link: https://resources.pcb.cadence.com/i/1180526
PSpice A/D User Guide Monte Carlo and sensitivity (worst-case) analyses October 2019 581 Product Version 17.4-2019 © 2022 All Rights Reserved. 2. Enter V2 in the Name text box. 3. Select Linear in the Sweep type frame. 4. Enter a 0 in the Start value text box. 5. Enter a 12 in the End value text box. 6. Enter a 1 in the Increment text box. PSpice A/D starts by running all of the analyses enabled in the Simulation Settings dialog box with all parameters set to their nominal values. However, with Monte Carlo enabled, PSpice A/D saves the DC sweep analysis results for later reference and comparison. After the nominal analyses are finished, PSpice A/D performs the additional specified analysis runs (in this example, DC sweep). Subsequent runs use the same analysis specification as the nominal run with one major exception: instead of using the nominal parameter values, the tolerances are applied to set new parameter values and thus, new part values. There is a trade-off in choosing the number of Monte Carlo runs. More runs provide better statistics, but they require more time. The amount of time scales directly with the number of runs: 20 transient analyses take 20 times as long as one transient analysis. During Monte Carlo runs, the PSpice A/D status display includes the current run number and the total number of runs left. Note: PSpice A/D offers a facility to generate histograms of data derived from Monte Carlo waveform families through the performance analysis feature. For information about performance analysis, see RLC filter example on page 525. For information about histograms, see Creating histograms on page 596. History support 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. However, at times users might want to keep some or all of the parameters similar for multiple analysis so that they can compare the results of multiple simulations.