开云体育

I have uploaded 2 files to the temp section that model a 120 degree
PTC thermistor, (the Epcos B59008C0120A040 from:
)
including the nonlinear behavior, modeled as 4 different temperature
coefficient resistors in series parallel.

The model is in file PTC1.asc
and the symbol is PTC_resistor.asy

The model also includes the internal temperature rise and thermal time
constant (which I guessed at, for lack of hard data). The symbol I
created for it has a third node that produces a voltage that
represents the internal temperature, with 1 volt = 1 degree C. The
curve across the resistor symbol indicates the 4 slopes in the model.

Everything I see this model doing looks pretty reasonable, but I would
appreciate anyone going over the whole thing and making suggestions
for improving it.

This was my first foray into model building with Spice.

--- In LTspice@..., "jpopelish" <jpopelish@r...> wrote:

I have uploaded 2 files to the temp section that model a 120 degree
PTC thermistor, (the Epcos B59008C0120A040 from:
)
including the nonlinear behavior, modeled as 4 different temperature
coefficient resistors in series parallel.

The model is in file PTC1.asc
and the symbol is PTC_resistor.asy

The model also includes the internal temperature rise and thermal
time constant (which I guessed at, for lack of hard data).
The symbol I created for it has a third node that produces a
voltage that represents the internal temperature, with
1 volt = 1 degree C. The curve across the resistor symbol
indicates the 4 slopes in the model.

Everything I see this model doing looks pretty reasonable, but I
would appreciate anyone going over the whole thing and making
suggestions for improving it.

This was my first foray into model building with Spice.

Hello John,

I did some first tests on your model and discovered that there is
a mistake in one of your formulas. I checked it with a temperature
sweep and the value of voltage source V1 set to 1mV DC.
.TEMP 10 250 1
Plot the resistance Rptc which is V/I: -1m/I(V1)

The given formula:
B1 1 2 I=V(1,2)/(.....+exp(H-(TK+V(4))*J)))

You have forgot the "TEMP" in the last exp() function.
It has been correct in your power disspiaton formula.

B1 1 2 I=V(1,2)/(exp(.....+exp(H-(TEMP+TK+V(4))*J)))

The resistance versus temperature agreed very well with
the datasheet.

Thanks for this model.
How did you calculate the 8 model paramaters?

Best regards,
Helmut

PS: I collect at the moment some literature about PTC models in
other SPICE programs. I will come back later with my results.

--- In LTspice@..., "Helmut Sennewald"
<helmutsennewald@y...> wrote:

--- In LTspice@..., "jpopelish" <jpopelish@r...> wrote:

I have uploaded 2 files to the temp section that model a 120 degree
PTC thermistor, (the Epcos B59008C0120A040 from:
)
including the nonlinear behavior, modeled as 4 different temperature
coefficient resistors in series parallel.

The model is in file PTC1.asc
and the symbol is PTC_resistor.asy

The model also includes the internal temperature rise and thermal
time constant (which I guessed at, for lack of hard data).
The symbol I created for it has a third node that produces a
voltage that represents the internal temperature, with
1 volt = 1 degree C. The curve across the resistor symbol
indicates the 4 slopes in the model.

(snip)

Hello John,

I did some first tests on your model and discovered that there is
a mistake in one of your formulas. I checked it with a temperature
sweep and the value of voltage source V1 set to 1mV DC.
.TEMP 10 250 1
Plot the resistance Rptc which is V/I: -1m/I(V1)

The given formula:
B1 1 2 I=V(1,2)/(.....+exp(H-(TK+V(4))*J)))

You have forgot the "TEMP" in the last exp() function.

Thank you. I think I have corrected this in the .asc file stored in temp.

It has been correct in your power disspiaton formula.

B1 1 2 I=V(1,2)/(exp(.....+exp(H-(TEMP+TK+V(4))*J)))

The resistance versus temperature agreed very well with
the datasheet.

Thanks for this model.
How did you calculate the 8 model paramaters?

I took resistance versus temperature as well as I could from the
graphical data on the data sheet. Then I manually approximated the 4
slopes graphically to get reasonable values. Then I ran a curve fit
program to find the minimum error fit of the combination of the 4
slopes to the data. The initial approximate solution is necessary
with my curve fit, because there are many local minima tthat are far
from the best solution. After getting my best fit, I looked at the
error of each point and fudged the data points a bit to achieve a
better fit which made the solution more stable. I justified this step
because the initial data was not actual measurements, but
approximations taken from a graph with a very fat line.

I might get a better fit if I used actual measurements, but, since I
would have no way of knowing how that device fit within the normal
manufacturing tolerances, that model would represent accurately, onlt
that single device. Unfortunately, PTC devices are not as well
specified as NTC devuces sometimes are.

I will upload some images of parts of the Mathcad worksheet I used to
perform this fit to the temp file area, as well as the whole
worksheet, for those who have Mathcad.

--- In LTspice@..., "jpopelish" <jpopelish@r...> wrote:

--- In LTspice@..., "Helmut Sennewald"
<helmutsennewald@y...> wrote:

--- In LTspice@..., "jpopelish" <jpopelish@r...>

wrote:

I have uploaded 2 files to the temp section that model a 120
degree PTC thermistor, (the Epcos B59008C0120A040 from:
)
including the nonlinear behavior, modeled as 4 different
temperature coefficient resistors in series parallel.

The model is in file PTC1.asc
and the symbol is PTC_resistor.asy

The model also includes the internal temperature rise and
thermal time constant (which I guessed at, for lack of hard
data).
The symbol I created for it has a third node that produces a
voltage that represents the internal temperature, with
1 volt = 1 degree C. The curve across the resistor symbol
indicates the 4 slopes in the model.

(snip)

Hello John,

I did some first tests on your model and discovered that there is
a mistake in one of your formulas. I checked it with a temperature
sweep and the value of voltage source V1 set to 1mV DC.
.TEMP 10 250 1
Plot the resistance Rptc which is V/I: -1m/I(V1)

The given formula:
B1 1 2 I=V(1,2)/(.....+exp(H-(TK+V(4))*J)))

You have forgot the "TEMP" in the last exp() function.

Thank you. I think I have corrected this in the .asc file
stored in temp.

It has been correct in your power disspiaton formula.

B1 1 2 I=V(1,2)/(exp(.....+exp(H-(TEMP+TK+V(4))*J)))

The resistance versus temperature agreed very well with
the datasheet.

Thanks for this model.
How did you calculate the 8 model paramaters?

I took resistance versus temperature as well as I could from the
graphical data on the data sheet. Then I manually approximated
the 4 slopes graphically to get reasonable values. Then I ran a
curve fit program to find the minimum error fit of the combination
of the 4 slopes to the data. The initial approximate solution is
necessary with my curve fit, because there are many local minima
tthat are far from the best solution. After getting my best fit,
I looked at the error of each point and fudged the data points a
bit to achieve a better fit which made the solution more stable.
I justified this step because the initial data was not actual
measurements, but approximations taken from a graph with a very
fat line.

I might get a better fit if I used actual measurements, but, since I
would have no way of knowing how that device fit within the normal
manufacturing tolerances, that model would represent accurately,
onlt that single device. Unfortunately, PTC devices are not as
well specified as NTC devuces sometimes are.

I will upload some images of parts of the Mathcad worksheet I used
to perform this fit to the temp file area, as well as the whole
worksheet, for those who have Mathcad.

Hello John,

I have already made a new folder with two sub-folders for the PTC
models.

Files > Lib > PTC Thermistors > Behaviorial Model

I recommend that you upload all your files into the folder above.
If you think you have a better name for your folder then feel free
to create one below the folder "Files > Lib > PTC Thermistors".

Best regards,
Helmut


PS: I am working on a model from Timo Veijola.
"Large-Signal Simulation Model for PTC Thermistor"

Extracting the paramters for new devices looks difficult, but
it's one of the very few sources about PTC resistors.
I hope that I can upload this model tomorrow.

This PTC-model is also used in TINA-Spice. They have some models
of PTCs(Philips?) in their demo version.

--- In LTspice@..., "Helmut Sennewald"
<helmutsennewald@y...> wrote:

Hello John,

I have already made a new folder with two sub-folders for the PTC
models.

Files > Lib > PTC Thermistors > Behaviorial Model

I recommend that you upload all your files into the folder above.
If you think you have a better name for your folder then feel free
to create one below the folder "Files > Lib > PTC Thermistors".

Best regards,
Helmut


PS: I am working on a model from Timo Veijola.
"Large-Signal Simulation Model for PTC Thermistor"

Extracting the paramters for new devices looks difficult, but
it's one of the very few sources about PTC resistors.
I hope that I can upload this model tomorrow.

This PTC-model is also used in TINA-Spice. They have some models
of PTCs(Philips?) in their demo version.

Thank you for the additional information.

I put both the model and component in the directory you created and
added a sub directory to cover the Mathcad derivation I used, in case
someone wants to reconstruct the method. Let me know if this is
appropriate. Once I have found home for this info, I guess I will
delete the files from the temp directory.

--- In LTspice@..., "jpopelish" <jpopelish@r...> wrote:

--- In LTspice@..., "Helmut Sennewald"
<helmutsennewald@y...> wrote:

Hello John,

I have already made a new folder with two sub-folders for
the PTC
models.

Files > Lib > PTC Thermistors > Behaviorial Model

I recommend that you upload all your files into the folder above.
If you think you have a better name for your folder then feel
free to create one below the folder
"Files > Lib > PTC Thermistors".

Best regards,
Helmut


PS: I am working on a model from Timo Veijola.
"Large-Signal Simulation Model for PTC Thermistor"

Extracting the paramters for new devices looks difficult, but
it's one of the very few sources about PTC resistors.
I hope that I can upload this model tomorrow.

This PTC-model is also used in TINA-Spice. They have some models
of PTCs(Philips?) in their demo version.

Thank you for the additional information.

I put both the model and component in the directory you created and
added a sub directory to cover the Mathcad derivation I used, in
case someone wants to reconstruct the method.
Let me know if this is appropriate. Once I have found home for
this info, I guess I will delete the files from the temp directory.

Hello John,

thanks for moving your files into this "Lib"-directory.
If your files in the "Temp"-folder are the same , then please
delete it from the Temp-folder.

I have finished today a model based on a work from Timo Veijola.

"Large-Signal Simulation Model for PTC Thermistor"


Extracting the paramters for new devices looks difficult, but
it's one of the very few sources about PTC resistors.

Files > Lib > PTC Thermistors > Physical model

What's about the idea of a more simple PTC-model just made of
a NTC resistor and a PTC resistor in series and one high value
ohmic resistor in parallel to both? It would only require 5
parameters, maybe with an optional parameter for some voltage
dependency.

Best regards,
Helmut


PS:
This PTC-model is also used in TINA-Spice.
They have some models of PTCs(Philips) in their demo version.

The parameters are fully compatible to the mentioned article
from Timo Veijola.


Another resource about PTCs is in the document
"General Technical Information" on the webpages from www.epcos.com


earResistors/PTCThermistors/SwitchingApplications/Page,templateId=ren
der,locale=en.html

Hello Helmut,

I have finished today a model based on a work from Timo Veijola.
...
Files > Lib > PTC Thermistors > Physical model

Looks impressive, hope I'll find the time to have a closer look at it!
There is one file missing: ptc_phil1.lib.

regards,
gerd

--- In LTspice@..., "gxxmxx" <gmildner@t...> wrote:

Hello Helmut,

I have finished today a model based on a work from Timo Veijola.
...
Files > Lib > PTC Thermistors > Physical model

Looks impressive, hope I'll find the time to have a closer look at it!
There is one file missing: ptc_phil1.lib.

regards,
gerd

Hello Gerd,

Thanks for the hint about the missing model file. I have uploaded
this file now.

It's helpful to read the mentioned article "ptc99.pdf" from Timo
Veijola.

Best regards,
Helmut

--- In LTspice@..., "Helmut Sennewald"
<helmutsennewald@y...> wrote:
(snip)

What's about the idea of a more simple PTC-model just made of
a NTC resistor and a PTC resistor in series and one high value
ohmic resistor in parallel to both? It would only require 5
parameters, maybe with an optional parameter for some voltage
dependency.

(snip)

For many applications, like limit temperature sensing, it should work
fine. In fact, it would make little difference for non self heating
applications if you skip the parallel constant resistance. The main
need for the high temperature negative temperature coefficient part of
the model is for over current limit applications, where you approach
the voltage limit of the device and self heating is severe so thermal
run away is a possibility. But a more general model works for
everything and doesn't leave you wondering if the model is telling you
the truth (or at least as much truth as the data sheet might contain).

Data sheets are so generally so poor (especially for devices intended
as current limiters), that I suspect that most people who go to the
trouble of fitting a model to a device may also have to go to the
trouble of measuring their own temperature resistance data, so the
added effort to fit a few extra segments is a trivial additional bit
of work, by the time they get that far.

At this point, my main interest, besides learning the rudiments of
spice modeling syntax, was to see what kind of math could efectively
model a typical PTC device. I found several other kind of functions
(e.g. combinations of exponentials of various powers of temperature,
rather than combinations of exponentials of linear functions of
temperature) that work well, but they are not as easy to explain as
the one I posted in the Mathcad document.

I would be very happy for this effort if we could just get the
manufacturers to supply a simple table of resistance cversus
temperature for their PTC thermistors, including tolerance, like many
do for NTC thermistors. Typical thermal resistance to ambient and
thermal mass would also be nice. What the heck, why don't they
provide Spice models?

Hi John:

You wrote:
>At this point, my main interest, besides learning the rudiments of
>spice modeling syntax, was to see what kind of math could efectively
>model a typical PTC device. ?I found several other kind of functions
>(e.g. combinations of exponentials of various powers of temperature,
>rather than combinations of exponentials of linear functions of
>temperature) that work well, but they are not as easy to explain as
>the one I posted in the Mathcad document.

You might be interested in two programs I found:
1) Tracer
This program allows you to cut a graph from another Windows program (ie, web browser, PDF file, scanned picture) & paste it into this program. ?After telling it where the corners of the graph are, you can trace the curve to get ?a set of discrete datapoints for curve-fitting. ?I found this program to be worth it's weight in gold, due to time saved transcribing graphs.
Find it at http://www.geocities.com/karolewski/soft.htm

2) CurveExpert
You can paste a series of X-Y datapoints into this program, then ask it to find the best formula to fit the data from a collection of dozens of standard formulas. ?User formulas are supported as well.
The Tracer web page also mentions a curve-fitting tool named PeakFitter. I tried both CurveExpert and PeakFitter, and liked CurveExpert a little better. YMMV.

Pat

Resent with missing link.

Hi John:

You wrote:
>At this point, my main interest, besides learning the rudiments of
>spice modeling syntax, was to see what kind of math could efectively
>model a typical PTC device. ?I found several other kind of functions
>(e.g. combinations of exponentials of various powers of temperature,
>rather than combinations of exponentials of linear functions of
>temperature) that work well, but they are not as easy to explain as
>the one I posted in the Mathcad document.

You might be interested in two programs I found:
1) Tracer
This program allows you to cut a graph from another Windows program (ie, web browser, PDF file, scanned picture) & paste it into this program. ?After telling it where the corners of the graph are, you can trace the curve to get ?a set of discrete datapoints for curve-fitting. ?I found this program to be worth it's weight in gold, due to time saved transcribing graphs.
Find it at http://www.geocities.com/karolewski/soft.htm

2) CurveExpert
You can paste a series of X-Y datapoints into this program, then ask it to find the best formula to fit the data from a collection of dozens of standard formulas. ?User formulas are supported as well.
It's at http://home.comcast.net/~curveexpert/
The Tracer web page also mentions a curve-fitting tool named PeakFitter. I tried both CurveExpert and PeakFitter, and liked CurveExpert a little better. YMMV.

Pat

--- In LTspice@..., pat_lawler@c... wrote:

Hi John:

You might be interested in two programs I found:
1) Tracer
This program allows you to cut a graph from another Windows program

(ie,

web browser, PDF file, scanned picture) & paste it into this program.
After telling it where the corners of the graph are, you can trace the
curve to get a set of discrete datapoints for curve-fitting. I found
this program to be worth it's weight in gold, due to time saved
transcribing graphs.
Find it at

2) CurveExpert
You can paste a series of X-Y datapoints into this program, then ask

it to

find the best formula to fit the data from a collection of dozens of
standard formulas. User formulas are supported as well.
The Tracer web page also mentions a curve-fitting tool named

PeakFitter. I

tried both CurveExpert and PeakFitter, and liked CurveExpert a little
better. YMMV.

Thanks for some very useful suggestions. I do a lot of curve fitting
for various enginnering purposes.