Issue link: https://resources.pcb.cadence.com/i/1180526
PSpice User Guide Mixed analog/digital simulation October 2019 640 Product Version 17.4-2019 © 1999-2019 All Rights Reserved. Interconnecting analog and digital parts Prior to simulation, netlisting translates the part instances and nets defined in your schematic into parts connected by nodes. The standard simulation netlist contains a flat view of the circuit. You can also create hierarchical netlists. PSpice A/D extracts the definitions for all parts modeled as subcircuits, viewing parts as a collection of primitive parts and node connections. The digital primitives that make up a digital part determine the way that PSpice A/D processes an analog/digital interface to that part. Specifically, the I/O model for each digital primitive connected at the interface gives PSpice A/D the necessary information. PSpice A/D recognizes three types of nodes: analog nodes, digital nodes, and interface nodes. The node type is determined by the types of parts connected to it. If all of the parts connected to a node are analog, then it is an analog node. If all of the parts are digital, then it is a digital node. If there is a combination of analog and digital parts, then it is an interface node. PSpice A/D automatically breaks interface nodes into one purely analog and one or more digital nodes by inserting one or more analog/digital interface subcircuits. PSpice A/D also automatically connects a power supply to the interface subcircuit to complete the generation of the interface. To view simulation results at an analog/digital interface in your schematic using the graphical waveform analyzer: ■ Place a marker on the appropriate interface net. The additional nodes created by PSpice A/D remain transparent. ■ View results in PSpice A/D by selecting traces from the output variable list (from the Trace menu, choose Add Trace). If you use this approach, note the names PSpice A/D generates for the new nodes. To find out more, see Interface generation and node names on page 651.