Measure impedance with spice cad program?

R

rob

Guest
Hi to all.
I was wondering if it is possible to measure impedances directly with
programs
like LTspice or Orcad.
For instance:
When simulating a class a small sig amp I would like to be
able to click on the base and have the simulator show the input
impedance.
You can measure voltage and current no problem , so I assume there
should be a way to show impedance.
Cheers
Rob
 
rob wrote:
Hi to all.
I was wondering if it is possible to measure impedances directly with
programs
like LTspice or Orcad.
For instance:
When simulating a class a small sig amp I would like to be
able to click on the base and have the simulator show the input
impedance.
Click to expand...
I don't think any Spices are that easy. You generally have to do a
manually set-up of V/I.

In SuperSpice, you can use the AC sweep set-up to specify a source as an
impedance source, and it will automatically do a plot of input/output
impedance at that point without any other setting up. There is an
example impedance.sss.

Its a nice idea, I might add it in. SuperSpice does do this already for
power, that is alt-clicking on the device will plot is power.

Kevin Aylward
salesEXTRACT@anasoft.co.uk
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.
 
On 12 Sep 2003 05:05:16 -0700, seegoon99@yahoo.com (rob) wrote:

Hi to all.
I was wondering if it is possible to measure impedances directly with
programs
like LTspice or Orcad.
For instance:
When simulating a class a small sig amp I would like to be
able to click on the base and have the simulator show the input
impedance.
You can measure voltage and current no problem , so I assume there
should be a way to show impedance.
Cheers
Rob
Click to expand...
For *impedance* force an unit AC current into the node, then display
Real and Imaginary parts of the resultant voltage.

For *admittance* force an unit AC voltage onto the node, then display
Real and Imaginary parts of the resultant current.

...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.
 
Hi,

I was wondering if it is possible to measure impedances directly with
programs
like LTspice or Orcad.
For instance:
When simulating a class a small sig amp I would like to be
able to click on the base and have the simulator show the input
impedance.
Click to expand...
TINA PRO has a facility for directly reading the real or complex
impedance of a circuit node. Their URL is -

http://www.tina.com/


Cheers - Joe
 
Rob,

I will need to create a model of a semiconductor device based upon its
physics -- that is, based upon the constituitive relations,
depletion lengths, Fermi levels, and all that other junk you find in
Sze. I am probably going to do it using an XSpice codemodel.

I am kind of confused about how I can model the C(V) behavior
of the device, because as far as I know the IOs provided by a
codemodel only allow you to input/output voltages and/or currents,
and I don't know how to put in time information (i.e. to support
the differentiating behavior of the cap).
Click to expand...
It's probably much easier to just write this type of spice device
without using xspice. That's been my experience anyway. Integration
of the general non-linear capacitance isn't too hard to figure
out. LTspice has an arbitrary capacitance device that is useful for
rapid prototyping new charge models. I'm not much of a fan of xspice
and I have not seen it used by the major SPICE programs like LTspice,
PSpice, hspice, or Spectre.

Is anybody here aware of a good text-book which would illuminate
the internal workings of SPICE, and provide a guide to extending it
using XSpice codemodels? I have looked at a few on-line theses and
such, but I need something more like "codemodels for dummies".
Click to expand...
There's various books on how SPICE works, the 2nd edition of the one
JT suggests is one I always recommend and you will need, but doesn't
address SPICE internals. A good one there is the one by Pillage and
Rohrer. I've been thinking of writing one myself, but until then
you should just get every one you can find if you want to get involved
in this. It's a interesting endeavor. You'll find yourself in club
smaller than the number of people that walked on the moon.

--Mike
 
"Mike Engelhardt" <pmte@concentric.net> wrote in message news:<bjspt1$oot@dispatch.concentric.net>...
Rob,

I will need to create a model of a semiconductor device based upon its
physics -- that is, based upon the constituitive relations,
depletion lengths, Fermi levels, and all that other junk you find in
Sze. I am probably going to do it using an XSpice codemodel.

I am kind of confused about how I can model the C(V) behavior
of the device, because as far as I know the IOs provided by a
codemodel only allow you to input/output voltages and/or currents,
and I don't know how to put in time information (i.e. to support
the differentiating behavior of the cap).

It's probably much easier to just write this type of spice device
without using xspice. That's been my experience anyway. Integration
of the general non-linear capacitance isn't too hard to figure
out. LTspice has an arbitrary capacitance device that is useful for
rapid prototyping new charge models. I'm not much of a fan of xspice
and I have not seen it used by the major SPICE programs like LTspice,
PSpice, hspice, or Spectre.

Is anybody here aware of a good text-book which would illuminate
the internal workings of SPICE, and provide a guide to extending it
using XSpice codemodels? I have looked at a few on-line theses and
such, but I need something more like "codemodels for dummies".

There's various books on how SPICE works, the 2nd edition of the one
JT suggests is one I always recommend and you will need, but doesn't
address SPICE internals. A good one there is the one by Pillage and
Rohrer. I've been thinking of writing one myself, but until then
you should just get every one you can find if you want to get involved
in this. It's a interesting endeavor. You'll find yourself in club
smaller than the number of people that walked on the moon.

--Mike
Click to expand...
In Pspice/Schematics you can set both voltage and current probes at
the point where you want to measure impedance. For the real part of
the impedance you simply add a trace once you run the simulation
labelled V(x)/I(x) which will give you the resistance of the point
being probed. This is best done in an AC analysis which has the
advantage of showing you the frequency response of the real portion of
the impedance as well.

The next step is to run the same model with a voltage phase probe at
the measurement point. This is available in Schematics in "Markers",
"Mark advanced". This, for obvious reasons, only works with an AC
analysis. You will now have the resistance and phase, at all relevant
frequencies, from which you can calculate any other parameters.

This works in Pspice/Schematics. I don't know about other versions of
Spice, but I would assume something similar is available.

John
 
Captain794@yahoo.com (The Captain) wrote in message news:<7199d521.0309130613.1252113@posting.google.com>...
"Mike Engelhardt" <pmte@concentric.net> wrote in message news:<bjspt1$oot@dispatch.concentric.net>...
Rob,

I will need to create a model of a semiconductor device based upon its
physics -- that is, based upon the constituitive relations,
depletion lengths, Fermi levels, and all that other junk you find in
Sze. I am probably going to do it using an XSpice codemodel.

I am kind of confused about how I can model the C(V) behavior
of the device, because as far as I know the IOs provided by a
codemodel only allow you to input/output voltages and/or currents,
and I don't know how to put in time information (i.e. to support
the differentiating behavior of the cap).

It's probably much easier to just write this type of spice device
without using xspice. That's been my experience anyway. Integration
of the general non-linear capacitance isn't too hard to figure
out. LTspice has an arbitrary capacitance device that is useful for
rapid prototyping new charge models. I'm not much of a fan of xspice
and I have not seen it used by the major SPICE programs like LTspice,
PSpice, hspice, or Spectre.

Is anybody here aware of a good text-book which would illuminate
the internal workings of SPICE, and provide a guide to extending it
using XSpice codemodels? I have looked at a few on-line theses and
such, but I need something more like "codemodels for dummies".

There's various books on how SPICE works, the 2nd edition of the one
JT suggests is one I always recommend and you will need, but doesn't
address SPICE internals. A good one there is the one by Pillage and
Rohrer. I've been thinking of writing one myself, but until then
you should just get every one you can find if you want to get involved
in this. It's a interesting endeavor. You'll find yourself in club
smaller than the number of people that walked on the moon.

--Mike

In Pspice/Schematics you can set both voltage and current probes at
the point where you want to measure impedance. For the real part of
the impedance you simply add a trace once you run the simulation
labelled V(x)/I(x) which will give you the resistance of the point
being probed. This is best done in an AC analysis which has the
advantage of showing you the frequency response of the real portion of
the impedance as well.

The next step is to run the same model with a voltage phase probe at
the measurement point. This is available in Schematics in "Markers",
"Mark advanced". This, for obvious reasons, only works with an AC
analysis. You will now have the resistance and phase, at all relevant
frequencies, from which you can calculate any other parameters.

This works in Pspice/Schematics. I don't know about other versions of
Spice, but I would assume something similar is available.

John
Click to expand...

Thanks for the help guys
Rob
 
In article <890c3e4d.0309120405.1dc14ecc@posting.google.com>, rob
<seegoon99@yahoo.com> writes
Hi to all.
I was wondering if it is possible to measure impedances directly with
programs
like LTspice or Orcad.
For instance:
When simulating a class a small sig amp I would like to be
able to click on the base and have the simulator show the input
impedance.
You can measure voltage and current no problem , so I assume there
should be a way to show impedance.
Cheers
Rob
I also have an application for measuring the negative real part of the
Click to expand...
input resistance to the terminals of a crystal (or LC) one port
oscillator.
I measure the (complex) volt drop across a low value resistor placed
between a frequency swept signal source and the oscillator terminals; LT
spice did not like negative resistors but I managed to overcome this by
shunting with enough resistance to ensure the result was always
positive.
Pierce oscillators and similar exhibit a negative resistance maxima
dependent on the frequency and capacitor values, this provides a good
means of determining the max crystal esr
that can be made to oscillate.

--
ddwyer
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top