Subject: Re: Diode Modeling in SPICE

From: [email-masked]
Date: Fri, 14 May 1999 08:35:08 -0500

Silvia,

It's been a while since I did this work, so my memory might be a little rusty...

I remember extracting Is and n parameters from lab data for bipolar transistors
a few years ago; this is essentially the same measurement.  We put the data on a
log-log plot.  From the slope you can get n.  The y-axis intercept gives you Is.

Start with the diode equation:

I = Is * {exp [(Vq)/(nkT)] - 1}

If you assume the -1 is negligible and take the natural log of both sides,

ln(I) = ln(Is) + (qV/nkT)

You'll also need some way to measure T.  For a nice graph, see "The PN Junction
Diode," by Gerold Neudeck, Addison-Wesley, 1989, figure 4.7, section 4.2, page
83 in my copy.

I applaud you for your efforts.  I wish all my model providers did this kind of
work!

(Shameless plug for a committee I've been working on:  you can find some useful
information on making accurate IBIS datasheets and documenting your results.
Look under "accuracy" on the IBIS web page.  It's called the IBIS Accuracy Spec,
although nobody is interested in using it as a spec just yet.  It has some great
information on what kind of measurements you can make to validate the accuracy
of the models you provide.)

Greg Edlund
Advisory Engineer, Critical Net Analysis
IBM
3650 Hwy. 52 N, Dept. HDC
Rochester, MN 55901
[email-masked]

"Montoya, Silvia" <[email-masked]> on 05/13/99 06:50:24 PM

To:   "[email-masked]'" <[email-masked]>
cc:   "Montoya, Silvia" <[email-masked]> (bcc: Gregory R
      Edlund/Rochester/IBM)
Subject:  Diode Modeling in SPICE

Hello IBIS model makers !

   I have a 5V CMOS I/O tristate-able buffer I'm trying to model.  The IBIS
curves generated by s2ibis2 are a very good match
   to measured data  between 0.7v up to about 5.9v.  But between -5V to 0.7v
and  5.9v to 10v the curves deviate quite a bit.
   I've disabled the parasitic diodes in the nmos and pmos device models (
IS=0 ) and added n+ and p+ parasitic diodes to the
   netlist.  I've been playing with the n+ and p+ diode model (level 3)
parameters  ( n,  js, ivb, area,  pj  )  trying to match SPICE
   results to measured data  with limited success.

   Are there any suggestions for other model parameters to tweek, or maybe
there is something going on with the s2ibis2 SPICE
   sim limits/parameters I'm not aware of  ?

  Thanks,
  The time you spend helping me out is greatly appreciated !

   Silvia Montoya
  email : [email-masked]

---

From: Lynne Green <[email-masked]>
Date: Sat, 15 May 1999 12:03:51 -0700 (PDT)

Silvia -

Diode models are notoriously poor at covering both forward and reverse
directions.

Main things to play with are series resistance RS and breakdown
characteristics (BV and IKV).  Tune RS to get a better fit in the forward
direction.  Then the breakdown characteristics can be tuned to get a
better fit in the reverse direction.

If the diode goes into forward punchthrough (junction reaches entirely through
a bulk layer), you may need to do more than this.  That doesn't sound likely
here.

Lynne Green
HyperLynx

-----FW: <[email-masked]

Date: Thu, 13 May 1999 16:50:24 -0700
From: "Montoya, Silvia" <[email-masked]>
To: "[email-masked]" <[email-masked]>
Subject: Diode Modeling in SPICE
Cc: "Montoya, Silvia" <[email-masked]>

 
  Thanks, 

   Silvia Montoya       

--------------End of forwarded message-------------------------

----------------------------------
E-Mail: Lynne Green <[email-masked]>
Date: 15-May-99
Time: 11:56:01

This message was sent by XFMail
----------------------------------