alainstas
Published © GPL3+

Create a QSPICE model for NTC Thermistor

Use this procedure to create an accurate QSPICE model for a NTC thermistor, using standard parameters from the data sheet

BeginnerProtip30 minutes296
Create a QSPICE model for NTC Thermistor

Things used in this project

Hardware components

Vishay NTCS0805
×1

Software apps and online services

Microsoft Excel
QSPICE

Story

Read more

Schematics

NTC thermistor model in QSPICE based on excel file

input information in excel file and import the model text in QSPICE

Code

NTC thermistor netlist for exclusive use in QSPICE

Plain text
copy / paste and import automatically in QSPICE
* Temperature_as_voltage_driven_thermistor for a Vishay NTC thermistor						
* exclusive netlist for Qspice -  04/01/2025						
* electrical pins : Rn Rp/ temperature pin :Tambient (exponential delay of temperature with a response time "tau") 						
* for worst case scenario: sweep the parameters "TOLR" (tolerance on R(25°C) and "TOLB" (tolerance on the B slope) throughout the min and max values						
* for nominal case: include a spice directive : "TOLR= 0" and "TOLB=0"						
.SUBCKT NTCS0805E3103FHT Rn Rp Tambient						
Vsense Rn Rn1 0						
B1 Tntc 0 I=-abs((V(Rn1)-V(Rp))*I(Vsense))						
R1 Tambient Tntc {Rth}						
C1 Tntc 0 {Cth}						
BI2 Rn1 Rp R=if(V(Tntc)<25,{R25}*{TR}*exp({W*TB}+ {X*TB}*(1/(273.15+V(Tntc)))+{Y*TB}*(1/(273.15+V(Tntc)))**2 +{Z*TB}*(1/(273.15+V(Tntc)))**3),						
+ {R25}*{TR}*exp({A*TB}+ {B*TB}*(1/(273.15+V(Tntc)))+{C*TB}*(1/(273.15+V(Tntc)))**2 +{D*TB}*(1/(273.15+V(Tntc)))**3))						
.params: TOLR=1 TOLB=1						
+W=-12.741052737133						
+X=3256.04554711565						
+Y=295699.289009381						
+Z=-39920342.5006774						
+A=-20.3177362537059						
+B=11545.3462988253						
+C=-2698020.38841962						
+D=316602057.011168						
+R25=10000						
+ TR={1+TOLR/100}						
+ TB={1+TOLB/100}						
+ Cth =0.036						
+ Rth= 166.666666666667						
.IC V(Tntc)=25						
.ends						

Credits

alainstas
70 projects • 38 followers
product marketing engineer at Vishay. began to simulate in spice programs in 2014.

Comments