Subject: DC convergence

From: Linda Chu x3207 <[email-masked]> (by way of John Angulo <[email-masked]>)
Date: Tue, 05 Sep 2000 16:42:20 -0700

Hi,
When DC sweep range from -Vcc to Vcc*2 on the PULLUP/PULLDOWN
simulation, it has convergence problem. I try to use the alternative
method is to do an AC, but the SPICE-IBIS convertor doesn't recognize
the spice output format. So when it generated the IBIS model, it puts
out N/A in the current table. Is there anyone can help me on this?
thanks
linda

---

From: Dan Aleksandrowicz <[email-masked]>
Date: Wed, 06 Sep 2000 09:51:38 +0200

Hi Linda.

This problem is very common. Your solution, however, is misguided.

I have the same problem with spice models from Fab we use.
I assume that the problem originated when the transistors were
extracted to spice the voltage range was lower than the Vdd IO.

However, I have solved it in two methods.

First, if you know some C you can try to changed the S2Ibis software
to work in the opposite direction. I mean you can modify the C to
generate
a put1.spi that has a DC sweep from 2*Vdd -> -Vdd.

The second solution, which work fine with a modified S2Ibis software,
is to set the voltage range to a limited Vdd like 2.5V instead of 3.3V.
While acutely connecting the Vdd generated by the S2Ibis file to a
dummy node. And setting Vdd to the true value.
To do this you must set VDDtyp=VDDmin=VDDmax in the voltage
range s2i file. Then you will have to change the result manually.
The change is the shifting of the pullup table voltage.
This method is very limited. And consumes a lot of man power.
But some times it you only solution.

For more ideas you are welcome to contact me.

--
                \\|//
                (o o)
~~~~~~~~~~~~oOOo~(_)~oOOo~~~~~~~~~~~~~~~~~~~
Dan Aleksandrowicz
Galileo Technology
Mercaz Ofek 1   (Building B')
Northern Industrial Zone, LOD 71293,  ISRAEL
email:[email-masked]
Tel: +972 8 9247555    (-
     Ext. 324         |__|
Fax: +972 8 9247554   |__|
                     #|oo| |--|   ___
           _  _    |--|  | |  |\ |oo|)        /\
       __  \\ \\   |------------\| #|--\     _||-
   ____\ \__\\_\\__|_||_________________\___|   |__v-___
   \                                                   /
    \      "Smoke on the water. Fire in the sky."     /
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~

---

From: "Lynne Green" <[email-masked]>
Date: Wed, 6 Sep 2000 11:34:15 -0700

Linda-

Did you check for a non-zero DC series resistance in your diode model?
You can get convergence problems when the diode currents get large.

- Lynne

-----Original Message-----
From: Linda Chu x3207 (by way of John Angulo <[email-masked]>)
[mailto:[email-masked]]
Sent: Tuesday, September 05, 2000 4:42 PM
To: [email-masked]
Subject: DC convergence

Hi,

---

From: Al Davis <[email-masked]>
Date: Wed, 6 Sep 2000 12:03:05 -0700

On Tue, 05 Sep 2000, Linda Chu x3207 wrote:
> simulation, it has convergence problem. ...

I think the real problem is that your real chip would probably go up
in smoke if you tried to force -Vcc or Vcc*2 into its signal pin,
without any series resistance to limit the current.  Spice uses
non-convergence as a method of representing the smoke.

The best bet is to not sweep that far if it causes trouble, then fake
it by extending the slope in a straight line.  Ideally, I would say
to stop the curves where you run out of data, but some simulators do
not extend the curve properly.

In any case, be sure test the resulting IBIS model, to make sure it
makes sense, and realize that you may need to tweak it a bit.