.... (sorry, I hit the wrong key and posted the above without finishing)

THE PROBLEM:
Is that in the descriptions I have seen in the thermistor model, you do a sweep of the control voltage and not temperature.  So, if you want to see what the thermistor does over a range of say 0 to 50 degrees,  you sweep the control voltage from 0 to 50 volts.  You plot and just label the x axis as temperature rather than voltage.

Well,  with the BJT, you have to actually sweep real temperature.  It's model has temperature varying elements in it.

So I am left with sweeping two different things, temperature and control voltage in a nested sweep statement.

I NEED A THERMISTOR MODEL WHERE YOU SWEEP TEMPERATURE NOT VOLTAGE TO MAKE IT CHANGE.

does anyone know of one?

Hi, I know this is an old thread now but I had a similar need & found this board just this week while trying (and failing) to find a solution.

I've now solved it myself  & thought I'd share my solution which is to use an Arbitrary Behavioural Voltage Source combined with a 0V Voltage source as a current sensor like this:

.subckt ntc 1 2 Params: * these  provide sensible defaults
+ R0=10k,
+ Beta=7660,
+ Rpar=1T,
+ t0 = 25,
+ TK = 273.15

* Arbitrary Behavioural Voltage source is used to generate
* Voltage equal to the NTC resistance @ global temp (in °C)
* multiplied by the current passing through it
BTherm 1 3 V = I(Vsense) * R0 *  exp (Beta/(temp + TK) - Beta/(t0 + TK))

* Current sensor
Vsense 3 2 0

Rparallel 1 2 R = Rpar

.ends

If you make this a library, you can then add commercially available Thermistors, e.g.

* Vishay Surface Mount NTC0805E4 series 2k2 @ 25°C
.subckt 2381_615_13222 1 2
x1 1 2 ntc Params: R0=2k2 Beta=3680
.ends

and predefined linearised sensors such as

*Oil Temperature Sensor
.subckt OilTemp 1 2
x1 1 2 ntc Params: R0=50k Beta=1780 Rpar=18k
.ends

or you can just use the select "ntc" as SpiceModel and define the parameters as you need in the LTSpice Component Attribute Editor e.g. Value as "R0=15k" , Value2 as "Beta=4660", SpiceLine as "T0=0", SpiceLine2 as "Rpar=1k5"

The model is obviously a simple one, with no account taken of frequency response, self-heating, etc. but it's much faster to run in LTSpice than the EPCOS ntc models available online.

Hope this is useful to somebody!

Yes, I am aware of the group's existence but I'm not a member. Unfortunately, because of the wide range of available, non-work related groups, Google Groups are generally frowned upon by our corporate network "guardians" (that's the polite word).

Thanks for the suggestion, though!