Pspice experts wanted

S

Sascha Warneke

Guest
Hello friends, I have a question connected with a problem.

I would like to simulate a temperature-dependent resistance. But i
want not to simulate it over a temperatur range. I want to simulate it
with a fixed temperature (for ex. at 27°C)

As soon as current flows through the resistance it changes its
resistance value, by becoming smaller.

I want to simulate these effect.

The other thing is, that in case of a tolerance design (using Pspice
AA) i have to define the tolerances at the resistors values.

I am not a newbie regarding to Pspice simulation, but such a
simulation i have never done before.

Can please somebody help me ?
Maybe somebody of you have done this ?

Thank you really much

Regards
 
On 7 Oct 2003 22:54:27 -0700, SaschaWarneke@web.de (Sascha Warneke)
wrote:

Hello friends, I have a question connected with a problem.

I would like to simulate a temperature-dependent resistance. But i
want not to simulate it over a temperatur range. I want to simulate it
with a fixed temperature (for ex. at 27°C)

As soon as current flows through the resistance it changes its
resistance value, by becoming smaller.

I want to simulate these effect.

The other thing is, that in case of a tolerance design (using Pspice
AA) i have to define the tolerances at the resistors values.

I am not a newbie regarding to Pspice simulation, but such a
simulation i have never done before.

Can please somebody help me ?
Maybe somebody of you have done this ?

Thank you really much

Regards
Click to expand...
The following subcircuit models the behavior of a lamp as it warms up.
Perhaps you can modify it to suit your needs.

****
** SPELLMAN LAMP SUBCIRCUIT
*VO=NOMINAL OPERATING VOLTAGE
*IO=NOMINAL STEADY STATE OPERATING CURRENT
*RCOLD=FILAMEMT RESISTANCE MEASURED AT ROOM TEMP (300K)
*TAU=CURRENT TIME CONSTANT AFTER A 0 (zero) TO VO STEP IS APPLIED
..SUBCKT LAMP 1 2 PARAMS: VO=28 IO=25m RCOLD=112 TAU=22m TAMB=300
H1 6 0 VML 1
RH1 6 0 1
GP 0 4 VALUE={V(6)*V(1,2)}
*V(4,0) = FILAMENT TEMPERATURE IN KELVINS
RT 4 5 {300*(VO-IO*RCOLD)/(IO*IO*VO*RCOLD)}
CT 4 5 {TAU*IO*IO*VO*RCOLD/(300*(VO-IO*RCOLD))}
VAMB 5 0 {TAMB}
El 7 0 1 2 300
R1 7 0 1
E2 8 0 VALUE={V(4)*RCOLD}
R2 8 0 1
E3 10 0 7 9 10MEG
R3 10 0 1
E4 9 0 VALUE={V(8)*V(10)}
R4 9 0 1
GR 1 3 10 2 1
VML 3 2 0
..ENDS LAMP
****

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
Jim Thompson wrote:

On 7 Oct 2003 22:54:27 -0700, SaschaWarneke@web.de (Sascha Warneke)
wrote:

Hello friends, I have a question connected with a problem.

I would like to simulate a temperature-dependent resistance. But i
want not to simulate it over a temperatur range. I want to simulate it
with a fixed temperature (for ex. at 27°C)

As soon as current flows through the resistance it changes its
resistance value, by becoming smaller.

I want to simulate these effect.

The other thing is, that in case of a tolerance design (using Pspice
AA) i have to define the tolerances at the resistors values.

I am not a newbie regarding to Pspice simulation, but such a
simulation i have never done before.

Can please somebody help me ?
Maybe somebody of you have done this ?

Thank you really much

Regards

The following subcircuit models the behavior of a lamp as it warms up.
Perhaps you can modify it to suit your needs.

****
** SPELLMAN LAMP SUBCIRCUIT
*VO=NOMINAL OPERATING VOLTAGE
*IO=NOMINAL STEADY STATE OPERATING CURRENT
*RCOLD=FILAMEMT RESISTANCE MEASURED AT ROOM TEMP (300K)
*TAU=CURRENT TIME CONSTANT AFTER A 0 (zero) TO VO STEP IS APPLIED
.SUBCKT LAMP 1 2 PARAMS: VO=28 IO=25m RCOLD=112 TAU=22m TAMB=300
H1 6 0 VML 1
RH1 6 0 1
GP 0 4 VALUE={V(6)*V(1,2)}
*V(4,0) = FILAMENT TEMPERATURE IN KELVINS
RT 4 5 {300*(VO-IO*RCOLD)/(IO*IO*VO*RCOLD)}
CT 4 5 {TAU*IO*IO*VO*RCOLD/(300*(VO-IO*RCOLD))}
VAMB 5 0 {TAMB}
El 7 0 1 2 300
R1 7 0 1
E2 8 0 VALUE={V(4)*RCOLD}
R2 8 0 1
E3 10 0 7 9 10MEG
R3 10 0 1
E4 9 0 VALUE={V(8)*V(10)}
R4 9 0 1
GR 1 3 10 2 1
VML 3 2 0
.ENDS LAMP
****

...Jim Thompson
About 12 years ago several grad students and I developed such a
Click to expand...
self-heating thermal model for a BJT, but we used the Watand simulator.
Watand allowed us to write link in subroutines in such ways to make it
happen.
Since that time I have continued an interest in this topic, but have
not yet had time to figure out if Spice can be easily modified to
accomplish this. It seems it cannot.
If you are interested, there were a few IEEE publications you might
be able to find, and I have seen a few newer items in the literature
which may help with this.
Unless thermal resistance and perhaps capacitance are included in
such a model, "self heating" is not really being modeled. J.Thompson's
idea looks more like a time-related model to vary the resistance. --Phil
--
Phil Munro Dept of Electrical & Computer Engin
mailto:pcMunro@cc.ysu.edu Youngstown State University
Youngstown, Ohio 44555
 
On Wed, 08 Oct 2003 11:55:07 -0400, Phil Munro <PcMunro@cc.ysu.edu>
wrote:

Jim Thompson wrote:

On 7 Oct 2003 22:54:27 -0700, SaschaWarneke@web.de (Sascha Warneke)
wrote:

Hello friends, I have a question connected with a problem.

I would like to simulate a temperature-dependent resistance. But i
want not to simulate it over a temperatur range. I want to simulate it
with a fixed temperature (for ex. at 27°C)

As soon as current flows through the resistance it changes its
resistance value, by becoming smaller.

I want to simulate these effect.

The other thing is, that in case of a tolerance design (using Pspice
AA) i have to define the tolerances at the resistors values.

I am not a newbie regarding to Pspice simulation, but such a
simulation i have never done before.

Can please somebody help me ?
Maybe somebody of you have done this ?

Thank you really much

Regards

The following subcircuit models the behavior of a lamp as it warms up.
Perhaps you can modify it to suit your needs.

****
** SPELLMAN LAMP SUBCIRCUIT
*VO=NOMINAL OPERATING VOLTAGE
*IO=NOMINAL STEADY STATE OPERATING CURRENT
*RCOLD=FILAMEMT RESISTANCE MEASURED AT ROOM TEMP (300K)
*TAU=CURRENT TIME CONSTANT AFTER A 0 (zero) TO VO STEP IS APPLIED
.SUBCKT LAMP 1 2 PARAMS: VO=28 IO=25m RCOLD=112 TAU=22m TAMB=300
H1 6 0 VML 1
RH1 6 0 1
GP 0 4 VALUE={V(6)*V(1,2)}
*V(4,0) = FILAMENT TEMPERATURE IN KELVINS
RT 4 5 {300*(VO-IO*RCOLD)/(IO*IO*VO*RCOLD)}
CT 4 5 {TAU*IO*IO*VO*RCOLD/(300*(VO-IO*RCOLD))}
VAMB 5 0 {TAMB}
El 7 0 1 2 300
R1 7 0 1
E2 8 0 VALUE={V(4)*RCOLD}
R2 8 0 1
E3 10 0 7 9 10MEG
R3 10 0 1
E4 9 0 VALUE={V(8)*V(10)}
R4 9 0 1
GR 1 3 10 2 1
VML 3 2 0
.ENDS LAMP
****

...Jim Thompson

About 12 years ago several grad students and I developed such a
self-heating thermal model for a BJT, but we used the Watand simulator.
Watand allowed us to write link in subroutines in such ways to make it
happen.
Since that time I have continued an interest in this topic, but have
not yet had time to figure out if Spice can be easily modified to
accomplish this. It seems it cannot.
If you are interested, there were a few IEEE publications you might
be able to find, and I have seen a few newer items in the literature
which may help with this.
Unless thermal resistance and perhaps capacitance are included in
such a model, "self heating" is not really being modeled. J.Thompson's
idea looks more like a time-related model to vary the resistance. --Phil
Click to expand...
I was modeling inrush currents in an aircraft lamp driver, but, if you
look closely, it *is* modeling self-heating.

Look up PSpice's "Device Equations" add-on to find out how to
add/change device models.

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
Jim Thompson wrote:

On Wed, 08 Oct 2003 11:55:07 -0400, Phil Munro <PcMunro@cc.ysu.edu
wrote:


Jim Thompson wrote:


On 7 Oct 2003 22:54:27 -0700, SaschaWarneke@web.de (Sascha Warneke)
wrote:


Hello friends, I have a question connected with a problem.

I would like to simulate a temperature-dependent resistance. But i
want not to simulate it over a temperatur range. I want to simulate it
with a fixed temperature (for ex. at 27°C)

As soon as current flows through the resistance it changes its
resistance value, by becoming smaller.

I want to simulate these effect.

The other thing is, that in case of a tolerance design (using Pspice
AA) i have to define the tolerances at the resistors values.

I am not a newbie regarding to Pspice simulation, but such a
simulation i have never done before.

Can please somebody help me ?
Maybe somebody of you have done this ?

Thank you really much

Regards

The following subcircuit models the behavior of a lamp as it warms up.
Perhaps you can modify it to suit your needs.

****
** SPELLMAN LAMP SUBCIRCUIT
*VO=NOMINAL OPERATING VOLTAGE
*IO=NOMINAL STEADY STATE OPERATING CURRENT
*RCOLD=FILAMEMT RESISTANCE MEASURED AT ROOM TEMP (300K)
*TAU=CURRENT TIME CONSTANT AFTER A 0 (zero) TO VO STEP IS APPLIED
.SUBCKT LAMP 1 2 PARAMS: VO=28 IO=25m RCOLD=112 TAU=22m TAMB=300
H1 6 0 VML 1
RH1 6 0 1
GP 0 4 VALUE={V(6)*V(1,2)}
*V(4,0) = FILAMENT TEMPERATURE IN KELVINS
RT 4 5 {300*(VO-IO*RCOLD)/(IO*IO*VO*RCOLD)}
CT 4 5 {TAU*IO*IO*VO*RCOLD/(300*(VO-IO*RCOLD))}
VAMB 5 0 {TAMB}
El 7 0 1 2 300
R1 7 0 1
E2 8 0 VALUE={V(4)*RCOLD}
R2 8 0 1
E3 10 0 7 9 10MEG
R3 10 0 1
E4 9 0 VALUE={V(8)*V(10)}
R4 9 0 1
GR 1 3 10 2 1
VML 3 2 0
.ENDS LAMP
****
...Jim Thompson

About 12 years ago several grad students and I developed such a
self-heating thermal model for a BJT, but we used the Watand simulator.
Watand allowed us to write link in subroutines in such ways to make it
happen.
Since that time I have continued an interest in this topic, but have
not yet had time to figure out if Spice can be easily modified to
accomplish this. It seems it cannot.
If you are interested, there were a few IEEE publications you might
be able to find, and I have seen a few newer items in the literature
which may help with this.
Unless thermal resistance and perhaps capacitance are included in
such a model, "self heating" is not really being modeled. J.Thompson's
idea looks more like a time-related model to vary the resistance. --Phil


I was modeling inrush currents in an aircraft lamp driver, but, if you
look closely, it *is* modeling self-heating.

Look up PSpice's "Device Equations" add-on to find out how to
add/change device models.

...Jim Thompson
Ok, thanks. Perhaps I looked too quickly at what you did. I will
Click to expand...
give it more time, when I find some! :) On the other hand, I do not
see R changing wrt calculated power. I see "nominal" VO and IO.
We tried messing with Device Equs with v8 PSpice, but did not give
that enough time, either. And it did not look as if it would do what we
needed to do. --Phil
--
Phil Munro Dept of Electrical & Computer Engin
mailto:pcMunro@cc.ysu.edu Youngstown State University
Youngstown, Ohio 44555
 
"Sascha Warneke" <SaschaWarneke@web.de> schrieb im Newsbeitrag
news:1ed295d9.0310072154.6ac02801@posting.google.com...
Hello friends, I have a question connected with a problem.

I would like to simulate a temperature-dependent resistance. But i
want not to simulate it over a temperatur range. I want to simulate it
with a fixed temperature (for ex. at 27°C)

As soon as current flows through the resistance it changes its
resistance value, by becoming smaller.

I want to simulate these effect.

The other thing is, that in case of a tolerance design (using Pspice
AA) i have to define the tolerances at the resistors values.

I am not a newbie regarding to Pspice simulation, but such a
simulation i have never done before.

Can please somebody help me ?
Maybe somebody of you have done this ?
Click to expand...

Hello Sascha,
EPCOS offers such PSPICE models for all of their NTC-Resistors.
www.epcos.de
Follow the path (left side)on their internet page.
Tools für Entwickler->NTC Thermistoren Bibliothek PSPICE ..
Download the file. Rename it to ntc_psp.exe. It is a selfextracting
zip-file.

http://www.epcos.de/excelon/servlet/excelon/tools/xml/tools_d.xml?xslsheet=t
ools:/xsl/tools.xsl&bereich=Thermistoren

Best Regards
Helmut

PS: "Warum in die Ferne schweifen, wenn das Gute liegt so nah?"


Beginning of their original documentation:
------------------------------------------
1. NTC thermistor model

Development of an NTC model for the "Pspice Design Center" circuit
simulation program allows inclusion of NTC thermistors in the computer-aided
design of modern electronic circuits.
An NTC thermistor is modeled under Pspice by its R/T curve, its heat
capacity and its dissipation factor.
Fig. 1 shows the structure of its equivalent circuit, consisting of a
thermal and an electric circuit.
The electric circuit consists of a variable resistor R(TNTC), connected by
leads 1 and 2 to the circuit of the PSpice user. The voltage V12 corresponds
to the voltage momentarily applied to the NTC, and the current INTC to the
current flowing through it. The temperature TNTC calculated in the thermal
circuit defines the size of the resistance R(TNTC).
The thermal circuit consists of a voltage-controlled current source, a
variable resistance and a capacitance. The .......
 
On 7 Oct 2003 22:54:27 -0700, SaschaWarneke@web.de (Sascha Warneke)
wrote:

Hello friends, I have a question connected with a problem.

I would like to simulate a temperature-dependent resistance. But i
want not to simulate it over a temperatur range. I want to simulate it
with a fixed temperature (for ex. at 27°C)

As soon as current flows through the resistance it changes its
resistance value, by becoming smaller.

[snip]
Click to expand...

PSpice doesn't directly support self-heating effects in resistor
models.

However you can model what you want using the Analog Behavioral Model
blocks.

Consider thermal resistance to be a resistor driven by a current
source whose value is power (V*I) in your temperature-dependent
resistance. You'll need some capacitance in there to emulate mass
(and thermal time constant).

Then feedback the temperature rise into the equations for your
resistor.

A bit of Algebra, but you should be able to do it ;-)

(You can obtain a voltage proportional to ambient temperature using an
ABM with TEMP as a variable.)

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top