Issue link: https://resources.pcb.cadence.com/i/1180526
PSpice User Guide Transient analysis October 2019 552 Product Version 17.4-2019 © 1999-2019 All Rights Reserved. The QSTD model is defined as: .MODEL QSTD NPN( is=1e-16 bf=50 br=0.1 rb=50 rc=10 tf=.12ns tr=5ns + cje=.4pF pe=.8 me=.4 cjc=.5pF pc=.8 mc=.333 ccs=1pF va=50) Instead of using the DC sweep to look at the hysteresis, use the transient analysis, (Print Step = .01ms and Final Time = 2ms) sweeping VIN from -1.8 volts to -1.0 volts and back down to -1.8 volts, very slowly. This has two advantages: ■ it avoids convergence problems ■ it covers both the upward and downward transitions in one analysis After the simulation, in the Probe window in PSpice, the X axis variable is initially set to Time. By selecting X Axis Settings from the Plot menu and clicking on the Axis Variable button, you can set the X axis variable to V(1). Then use Add on the Trace menu to display V(7), and change the X axis to a user-defined data range from -1.8V to -1.0V (Axis Settings on the Plot menu). This plots the output of the Figure 12-4 Netlist for Schmitt trigger circuit. * Capture Netlist R_RIN 1 2 50 R_RC1 0 3 50 R_R1 3 5 185 R_R2 5 8 760 R_RC2 0 6 100 R_RE 4 8 260 R_RTH2 7 0 85 C_CLOAD 0 7 5PF V_VEE 8 0 dc -5 V_VIN 1 0 +PWL 0 -8 1MS -1.0V 2MS -1.8V R_RTH1 8 7 125 Q_Q1 3 2 4 QSTD Q_Q2 6 5 4 QSTD Q_Q3 0 6 7 QSTD Q_Q4 0 6 7 QSTD