Simulating a variable resistance input with LTSpice?

Surprise! Three point subcircuit fit, R0 (nominal at 25°C) and at the end points of the data (same as above)... generates a Steinhart-Hart equation accurate to ±0.3%....

• PARAMS: R0=470 T0=25 R1=26618 T1=-55 R2=23.24 T2=125 .PARAM TK0={T0+273.15} .PARAM TK1={T1+273.15} .PARAM TK2={T2+273.15} .PARAM K01={TK0*TK1/(TK0-TK1)} .PARAM K02={TK0*TK2/(TK2-TK0)} .PARAM Q01={(TK0**3-TK1**3)/(TK0**3)/(TK1**3)} .PARAM Q02={(TK2**3-TK0**3)/(TK0**3)/(TK2**3)} .PARAM C={(K02*LOG(R0/R2)-K01*LOG(R1/R0))/((Q02*K02)-(Q01*K01))} .PARAM B={K01*LOG(R1/R0)-C*K01*Q01} .PARAM A={(-1)*(B/TK0+C/(TK0**3))} .PARAM TK={TEMP+273.15} .PARAM RT={R0*EXP(A+B/TK+C/(TK**3))} G_G1 THERMP THERMN VALUE {V(THERMP,THERMN)/RT} .ENDS ThermistorSH3PT

(Math all solved by PSpice within the subcircuit declaration :-) ...Jim Thompson