You can simulate an NTC thermistor in NI Multisim™, but you cannot use the RESISTOR_VIRTUAL component because its temperature model is intended to represent a resistance temperature detector (RTD), whose resistance increases with temperature.
-
To create an NTC thermistor model:
-
Open Tools>>Component Wizard and create a new custom component.
-
-
In the Select Simulation Model step, define a resistor model that follows the resistance-versus-temperature behavior of an NTC thermistor. For example, the following SPICE subcircuit models a 1 kΩ thermistor using two known resistance-temperature points:
- T0 = 20 °C, R0 = 1 kΩ
- T1 = 120 °C, R1 = 55 Ω
.SUBCKT 1KOHM_NTC_THERMISTOR 1 2 PARAMS: T0=20 R0=1k T1=120 R1=55 R1 1 2 R0*((R1/R0)^((T0*T1-TEMP*T1)/(TEMP*T0-TEMP*T1)))
.ENDS
Additional Information
Why can't RESISTOR_VIRTUAL be used as an NTC thermistor?
The RESISTOR_VIRTUAL component uses an RTD temperature model defined by the parameters TC1, TC2, and TNOM:
This equation models devices whose resistance increases with temperature. While negative values for TC1 or TC2 may appear to produce a decreasing resistance over a limited temperature range, the model is based on a polynomial RTD approximation and does not accurately represent the exponential resistance-versus-temperature characteristic of an NTC thermistor.
How does an NTC thermistor behave?
An NTC thermistor exhibits a nonlinear temperature response in which the resistance decreases as temperature increases. A common thermistor model is:
where:
- R(T) is the resistance at temperature T.
- K0 and b are thermistor-specific constants.
When two resistance-temperature pairs are known, the thermistor equation can be rewritten as:
where:
- T0, R0 represent the first temperature-resistance pair.
- T1, R1 represent the second temperature-resistance pair.
The SPICE model shown in Step 3 implements this equation, allowing the custom component to reproduce the expected NTC thermistor behavior over temperature more accurately than the built-in RTD-based resistor model.