Issue link: https://resources.pcb.cadence.com/i/1180526
PSpice User Guide Convergence and "time step too small errors" October 2019 837 Product Version 17.4-2019 © 1999-2019 All Rights Reserved. ■ Derivatives in PSpice are limited to 1e14. ■ The arithmetic used in PSpice is double precision and has 15 digits of accuracy. Is there a solution? Yes, for any physically realistic circuit. However, it is not difficult to set up a circuit that has no solution within the limits of PSpice numerics. Consider, for example, a voltage source of one megavolt connected to a resistor of one micro-ohm. This circuit does not have a solution within the dynamic range of currents (+/- 1e10 amps). Here is another example: V1 1, 0 5v D1 1, 0 DMOD .MODEL DMOD(IS=1e-16) The problem here is that the diode model has no series resistance. To find out more about the diode equations, refer to the Analog Devices chapter in the online PSpice Reference Guide. It can be shown that the current through a diode is: I = IS*e V/(N*k*T/q) N defaults to one and k*T at room temperature is about .025 volts. So, in this example the current through the diode would be: I = 1e-16*e 200 = 7.22e70 amps This circuit also does not have a solution within the limits of the dynamic range of PSpice. In general, be careful of components without limits built into them. Extra care is needed when using the expressions for controlled sources (such as for behavioral modeling). It is easy to write expressions with very large values. Are the equations continuous? The device equations built into PSpice are continuous. The functions available for behavioral modeling are also continuous (there are several functions, such as int(x), which cannot be added because of this). So, for physically realistic circuits the equations can also be continuous. Exceptions that come are usually from exceeding the