Issue link: https://resources.pcb.cadence.com/i/1180526
PSpice A/D User Guide Digital device modeling October 2019 411 Product Version 17.4-2019 © 2022 All Rights Reserved. libraries, describes how to translate a digital state into a voltage and impedance. .model DIN74 dinput ( + s0name="0" s0tsw=3.5ns s0rlo=7.13 + s0rhi=389 ; 7ohm, 0.09v + s1name="1" s1tsw=5.5ns s1rlo=467 + s1rhi=200 ; 140ohm, 3.5v + s2name="X" s2tsw=3.5ns s2rlo=42.9 + s2rhi=116 ; 31.3ohm, 1.35v + s3name="R" s3tsw=3.5ns s3rlo=42.9 + s3rhi=116 ; 31.3ohm, 1.35v + s4name="F" s4tsw=3.5ns s4rlo=42.9 + s4rhi=116 ; 31.3ohm, 1.35v + s5name="Z" s5tsw=3.5ns s5rlo=200K + s5rhi=200K +) The DINPUT model parameters are described under PSpice N devices in the PSpice A/D Reference Guide. Each state is turned into a pullup and pulldown resistor pair to provide the correct voltage and impedance. The Z state is accounted for as well as the 0, 1, and X logic levels. You can create your own interface subcircuits, DINPUT models, DOUTPUT models, and I/O models like these for technologies not currently supported in the model libraries. We recommend that you save these in your own custom model library, which you can then configure for use with a given design.