Understanding SPICE model devices

A

AJ

Guest
I am trying to create a device model for a small signal diode. The
problem is, I don't know how to translate real world specs into the
numbers that SPICE wants. The most useful piece of information to me
right now, is what Area Factor means, but I can't seem to get a
straight answer out of the internet on that one. Sure, a lot of sites
talk about it, but they don't say what it *is* or how to calculate it.

I know this is a pretty basic thing, but I am totally new to circuit
simulation. I figure that the combination of Area Factor, and one of
the other numbers inside the model determine the basic characteristics
of the diode, but I don't know how.

Any starting hints?
 
AJ wrote:
I am trying to create a device model for a small signal diode.
Click to expand...
What device is it? Most models already exist on manufacture web sites.

The
problem is, I don't know how to translate real world specs into the
numbers that SPICE wants. The most useful piece of information to me
right now, is what Area Factor means, but I can't seem to get a
straight answer out of the internet on that one. Sure, a lot of sites
talk about it, but they don't say what it *is* or how to calculate it.
Click to expand...
It is a simple multiplier that you use when you put identical devices in
parallel, more or less. For most models just ignore it, i.e. it defaults
to 1.

I know this is a pretty basic thing, but I am totally new to circuit
simulation. I figure that the combination of Area Factor, and one of
the other numbers inside the model determine the basic characteristics
of the diode, but I don't know how.

Any starting hints?
Click to expand...
Find out if the model already exists first. A few spice vendors have
demos that include a model maker. I will leave it to you to find out
which ones. Hint: google.

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.

"That which is mostly observed, is that which replicates the most"
http://www.anasoft.co.uk/replicators/index.html

"quotes with no meaning, are meaningless" - Kevin Aylward.
 
I am trying to create a device model for a small signal diode.

What device is it? Most models already exist on manufacture web sites.
Click to expand...
It is a 1N60 germanium diode, which I guess you'd typically use in an
AM/FM detector. It's easy enough to take the reverse breakdown
volatage (40V) and the current at breakdown voltage and insert them
directly into the model, however, these are not the important numbers,
because my circuit is not going to send the diodes anywhere near
breakdown.

The only facts I have to go on are the the current at a forward
voltage of 0.05V, which is 0.375mA. So apart from that and the
breakdown characteristics, that's all I have to create the magic
numbers inside a diode model.


Any starting hints?

Find out if the model already exists first. A few spice vendors have
demos that include a model maker. I will leave it to you to find out
which ones. Hint: google.
Click to expand...
Well I was hoping to understand the variables inside the model format,
rather than have a piece of software build the model for me. The SPICE
documentation names the variables and goes almost nowhere in
explaining how they work.

AJ
 
AJ wrote:
I am trying to create a device model for a small signal diode.

What device is it? Most models already exist on manufacture web
sites.

It is a 1N60 germanium diode, which I guess you'd typically use in an
AM/FM detector. It's easy enough to take the reverse breakdown
volatage (40V) and the current at breakdown voltage and insert them
directly into the model, however, these are not the important numbers,
because my circuit is not going to send the diodes anywhere near
breakdown.

The only facts I have to go on are the the current at a forward
voltage of 0.05V, which is 0.375mA. So apart from that and the
breakdown characteristics, that's all I have to create the magic
numbers inside a diode model.
Click to expand...
"is" sets the Vd verses Id graph from

Id=is.exp(q.Vd/KT.N)

cjo sets the basic device capacitance. It varies with voltage. "tt" sets
the diffusion capacitance. "rs" is pretty obvious.

You can fiddle with N for LEDs if "is" gives way off wrong reverse
leakage. N=1 is usually good enough.

Run some sims and fiddle with the equations to get a match.

Any starting hints?

Find out if the model already exists first. A few spice vendors have
demos that include a model maker. I will leave it to you to find out
which ones. Hint: google.

Well I was hoping to understand the variables inside the model format,
rather than have a piece of software build the model for me. The SPICE
documentation names the variables and goes almost nowhere in
explaining how they work.
Click to expand...
There are spice books about, but still, what's the point? If you
understand the *basic* device physics, the above should be enough to
make a basic model. If you don't, I would stick to the canned software.


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.

"That which is mostly observed, is that which replicates the most"
http://www.anasoft.co.uk/replicators/index.html

"quotes with no meaning, are meaningless" - Kevin Aylward.
 
In article <387bcaab.0402210155.ce1191b@posting.google.com>, AJ wrote:
I am trying to create a device model for a small signal diode. The
problem is, I don't know how to translate real world specs into the
numbers that SPICE wants. The most useful piece of information to me
right now, is what Area Factor means, but I can't seem to get a
straight answer out of the internet on that one. Sure, a lot of sites
talk about it, but they don't say what it *is* or how to calculate it.

I know this is a pretty basic thing, but I am totally new to circuit
simulation. I figure that the combination of Area Factor, and one of
the other numbers inside the model determine the basic characteristics
of the diode, but I don't know how.

Any starting hints?
Click to expand...
I once tried to contact the developers of spice-opus ( you can do a
google search ) about this same problem. They suggested to use
optimization technuiqes. Spice-opus has that support except you have to
buy it. You can use other tools to do optimization, But it would not be
as fast as a native implimentation.

IMHO if you are trying to learn how to do it then it's ok to proceed to
read-up on optimazation and device modeling and parameter extraction
stuff, But if you just want the exact model for a specific problem then
it's not worth the trouble.


,Fernan
 
I'd suggest trying to get hold of a copy of Ron Kielkowski's 'SPICE
Practical Device Modeling' (McGraw-Hill, 1995) through your library. In it
he describes how to do just what you are trying to do. For example, for a
diode, a plot of log(I) vs V will give you IS, N and RS. It is easy to
manipulate I=Is*exp(qV/NkT) to get log(I)=qV/NkT+log(Is): so the gradient is
q/NkT, which'll give you N; the y-axis intercept is log(Is), hence Is; RS is
a little harder to describe - find that V where the straight-line portion of
the line intercepts the Imax level, i.e. the level for the biggest value of
measured I, then RS=(Vmax-this)/Imax. You'll then have a model which, for DC
analyses at least, will match your data. Other parameters for AC analyses
and things needing capacitances etc. can be extracted similarly if you have
the appropriate data/measurements. I find both Kielkowski's books to be very
good (but pricey...)

Tim

--
__________________________________________________________
Tim Stinchcombe

Cheltenham, Glos, UK

"AJ" <aj.usenetspam@serato.com> wrote in message
news:387bcaab.0402210155.ce1191b@posting.google.com...
I am trying to create a device model for a small signal diode. The
problem is, I don't know how to translate real world specs into the
numbers that SPICE wants. The most useful piece of information to me
right now, is what Area Factor means, but I can't seem to get a
straight answer out of the internet on that one. Sure, a lot of sites
talk about it, but they don't say what it *is* or how to calculate it.

I know this is a pretty basic thing, but I am totally new to circuit
simulation. I figure that the combination of Area Factor, and one of
the other numbers inside the model determine the basic characteristics
of the diode, but I don't know how.

Any starting hints?
Click to expand...
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top