Issue link: https://resources.pcb.cadence.com/i/1180526
PSpice User Guide Convergence and "time step too small errors" October 2019 842 Product Version 17.4-2019 © 1999-2019 All Rights Reserved. ❍ Make sure that no (groups of) nodes are isolated from ground by current sources and/or capacitors. ❑ "Voltage source or inductor loop" message: ❍ Make sure that there are no loops of only inductors and/or voltage sources. ■ Place the ground (node 0) somewhere in the circuit. Be careful when you use floating grounds (e.g. chassis ground); you may need to connect a large resistor from the floating node to ground. All nodes will be reported as floating if "0 ground" is not used. ■ Make sure that voltage/current generators use realistic values, and verify that the syntax is correct. ■ Make sure that dependent source gains are correct, and that E/G element expressions are reasonable. Verify that division by zero or LOG(0) cannot occur. ■ Make sure that there are no unrealistic model parameters; especially if you have manually entered the model into the netlist. ■ Avoid using digital components, unless really necessary. Initialize the nodes with valid digital value to ensure the state is not ambiguous. Modelling circuit components ■ Semiconductors The first consideration for semiconductors is to avoid physically unrealistic model parameters. As PSpice steps the power supplies up, it has to step carefully through the turn on transition for each device. In the diode example above, for the setting N=1e-6, the knee of the I-V curve would be too sharp for PSpice to maintain its continuity within the power supply step size limit of 1e-6. ■ Behavioral modeling expressions Range limits: Voltages and currents in PSpice are limited to the range +/- 1e10. Care must be taken that the output of expressions falls within this range. This is especially important when one is building an electrical analog of a mechanical, hydraulic or other type of system.