Hi everyone, I've a NTC thermistor and I'd like to change its response curve. Am I right in thinking the following: I can linearise the thermistor using a series resistor. A resistor in parallel will change the gain of the thermistor A resistor in series with the thermistor will change the offset of the thermistor.
Many thanks in advance
David
The equations are known. Just pull up the math package.
Rene
-- Ing.Buero R.Tschaggelar - http://www.ibrtses.com & commercial newsgroups - http://www.talkto.net
Visit
--------------------------------------------
David,
Usually, I think of a *parallel* resistor as the thermistor's linearizer. And a resistor in *series* with the thermistor (i.e. with the linearizing resistor in parallel with the whole series combination) will change the factor by which the temperature changes the overall resistance. (Think of the series resistor as making the thermistor, and its resistance change vs temp, a smaller percentage of their series combination). Another resistor can also be added in series with the entire parallel network, to obtain a desired total resistance.
A pretty good way to do what you want, that I've used recently, is to use LTSpice to get the thermistor parameters and to verify your linearization (or response-shaping) results. (Note that for an existing (on-hand) thermistor for which you don't have an LTSpice model, you could use actual resistances, measured at three temperatures, with the equation below, to linearize it.)
Do the following:
Download LTSpice (aka SwitcherCADIII) from
Go to
Go to the files section and get the ntc.lib file, which has lots of Spice models for Epcos thermistors (which are actually available to purchase, through Digikey.com), which also include self-heating effects. There are also some very good thermistor examples/tutorials, available there. (The ntc.lib file is, I assume, also available from Epcos' website.)
Make a thermistor test fixture, in LTSPice, with a voltage source (v1) driving your grounded thermistor (and, later, your thermistor/resistor network). You can use a 1-volt sine at 60 Hz for the voltage source.
Label the ungrounded (i.e. driven) node as "OUT". Plot V(out)/-I(V1). (i.e. Run it and then right-click on the axis label at the top and change it to V(out)/-I(V1). Then save your plot settings.)
Use a TRAN statement like: .tran 0 .0002 .0001 .00000001
Step the temperature through three equally spaced temperatures, over the range you want to linearize for, with a statement like: .STEP TEMP
0 50 25 (i.e. 0C to 50C in 25C steps).Put the desired thermistor (or thermistor with series resistor) in the circuit (i.e. from the voltage source to ground).
Run the simulation.
in if you need to. Place the mouse cursor where you want to measure and then read the resistance at the lower left.
Use the following equation to calculate the value of the parallel resistance that will linearize the thermistor's temperature response (for resistances measured at 0, 25, and 50 degC, as stated; but change the temps if needed):
Rp = (R0*R25 + R25*R50 - 2*R0*R50) / (R0 + R50 - 2*R25)
Put the calculated parallel resistance, Rp, in the circuit and re-run the simulation.
Verify that the response is what you need at each temperature.
If needed, add a resistor in series with the whole thing, to get a desired total resistance.
If you're trying to get a specific curve shape, or specific resistances at specific temps, you may have to iteratively tweak the resistor values and re-run the simulation.
If anyone would like a copy of my linearize_thermistor.asc LTSpice file (described above), email me (tomg at fullnet.com).
Regards,
Tom Gootee
--------------------------------------------
ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.