Issue link: https://resources.pcb.cadence.com/i/1180526
PSpice User Guide Parametric and temperature analysis October 2019 520 Product Version 17.4-2019 © 1999-2019 All Rights Reserved. To create the capacitor model in the schematic editor: 1. Place a CBREAK part. 2. Select it so that it is highlighted. 3. From the Edit menu, choose PSpice Model. 4. In the Model Text frame, enter the following: .model Cnln CAP(C=1 VC1=-0.01 VC2=0.05) 5. From the File menu, choose Save. Set up the circuit for a parametric AC analysis (sweep Vbias), and run PSpice. Include only the frequency of interest in the AC sweep. To display the results Use PSpice to display the capacitance calculated at the frequency of interest versus the stepped parameter. 1. Simulate the circuit. 2. Load all AC analysis sections. 3. From the Trace menu, choose Add Trace or click the Add Trace toolbar button . 4. Add the following trace expression: IMG(-I(Vin)/V(1,0))/(2*3.1416*Frequency) Or add the expression: CvF(-I(Vin)/V(1,0)) Where CvF is a macro which measures the effective capacitance in a complex conductance. Macros are defined using the Macros command on the Trace menu. The CvF macro should be defined as: CvF(G)= IMG(G)/(2*3.1416*Frequency) Note: -I(Vin)/V(1) is the complex admittance of the R-C branch; the minus sign is required for correct polarity. To use performance analysis to plot capacitance vs. bias voltage 1. From the Trace menu, choose Performance Analysis.