It is all about using either an exponential function or the Stienhart-Hart equation or some other analytical expression to model the resistance of the thermistor vs temperature. LTSpice has a couple of ways to make a resistance that is a function of some parameter, or of a node voltage or branch current.
I recently needed a thermistor to include in a temperature measurement system. I looked at the
US Sensor 104JG1F thermistor sold by Digikey. They have the resistance vs temperature data for that thermistor as an Excel file (see the .xls file under Datasheets) . I got the data, and used Excel's curve fitting (trendline) to get a fifth-order polynomial that fits the resistance vs temperature data for the temperature range I am interested in.
I put that polynomial into a variable resistance in LTSpice, and was able to model the behavior of a more complex circuit that had the simulated thermistor in it. R3 is the thermistor. Note how I vary it using the parameter Rt.
I have attached the LTSpice sim for you. Note that the independent variable of the simulation is the temperature in degC (.step param C 94 240 5). I convert that to degF, because my thermistor model is written in terms of F (.param F= (C*9/5) + 32).
The .param Rt = -1.46778E-08*F**5 +... expression is the polynomial I fit through the supplied RvsF data I got from the maker.
LTSpice and PSpice have common roots, so everything I show here should work there. Note I plot the thermistor resistance,:the expression (V(d)-V(b))/I(R3) = Rt is in Ohms, and is plotted vs degC.
The current in R12 is what this circuit varies with temperature. Not interesting to you, but it was to me...