Re: [SI-LIST] : HSPICE to QUAD models

Mark Nass (markn@rccorp.com)
Thu, 29 Jan 1998 09:45:41 -0800

At 12:09 AM 1/29/98 -0500, Adrianus Djohan wrote:
>Mark,
>
>In what part of the waveform are they different?? Transient part
>(rise/fall edges) or the dc level or both?? How much is the difference??

The model I built is a GTL buffer, Master Slave model with partial
drive high.
The largest difference is in the Rise/Fall times and signal strength.
The bufer I am haveing the problem with is a GTL buffer. The rise
time in HSPICE measured from the start of the wave, .4 V, to 1.2V
is .751 ns. In QUAD I measure 1.22ns. Then in the area from 1V to
1.4V I measure .563 in HSPICE & 1.34 in QUAD. I've tried this with
just the buffer and also with a 2" line. I get similiar results.
The second test condition I used was 4 loads connected to the line,
all the same buffer type. I drove with one of the buffers in the middle
of the line and looked at the signal at the buffer next to it. They were
way different in reflection times & signal amplitudes.
But when I use the 10290 the the rise and fall times were within 50ps.
The reflections in the multiple load case also looked similiar, The ringback
was about .1V more. Also the PVPT model, with the 1st 1.29ns of data
stripped out and the new time set to zero also looked close in both cases.

>If you are having problem with the dc level, here are some possible
>causes:
>1. The pullup and/or pulldown resistor value that you specify in SPI2MOD
> is not the same value to that you use in generating the pullup and/or
> pulldown data in HSPICE.

Both are 25 ohm.

>2. The pullup voltage that you specify in SPI2MOD is not the same value
> to that you use in HSPICE.

Both are 1.5 V

>2. The buffer might use a master-slave technique. If this is the case, you
> want to generate model seperately for each set of the output
> transistors. And then use the master-slave feature in QUAD to merge
> them into a single driver.

I am doing this, it also has a partail drive high.

>3. If the buffer uses some sort of voltage feedback control, you won't be
> able to model this accurately in any of behavioural level modeling
> (QUAD, IBIS).
>
>If you are having problem with the transient part:
>1. We found that adjusting pullup and pulldown resistor value such that
> the 2 waveforms don't overlap improve the resulting model quality.
>2. We found that SPI2MOD doesn't generate the PVPT correctly if the buffer
> has small voltage swing, feedback controlled edge rate, or significant
> edge rate difference between the pullup and the pulldown transistors.
> We have some luck with generating the PVPT manually, specially for
> cause #1 and #3.
>3. In general, we found that buffer with fast edge rate is easier to
> model. Fast part would yeild more accurate QUAD model than its slow
> model.
>4. Try putting the right value of input capacitance in SPI2MOD.

The value of capacitance had made no difference in the conversion, it
was just a number passed along into the QUAD model.
>
>That's all what I could think of. I hope it helps!!
>
>Sincerely,
>Adrianus
>
>--
>***********************************************************************
>** Adrianus Djohan **
>** Analog and Signal Integrity Engineer **
>** STRATUS COMPUTER **
>** Mail Stop: M3-2-EN3 email :Adrianus_Djohan@stratus.com **
>** 55 Fairbanks Boulevard phone : (508) 490-6611 **
>** Marlborough, MA 01752 fax : (508) 480-8219 **
>** USA **
>***********************************************************************
>
>
>On Wed, 28 Jan 1998, Mark Nass wrote:
>
>> Date: Wed, 28 Jan 1998 19:29:29 -0800
>> From: Mark Nass <markn@rccorp.com>
>> To: si-list@silab.Eng.Sun.COM
>> Subject: [SI-LIST] : HSPICE to QUAD models
>>
>> I have generated some QUAD models using HSPICE generated data. I used
>> the SPI2MOD program and have found some problems and wanted to know if
>> anybody has a similar experience, or a better method.
>> I got my rise/fall data, vol & voh data. With SPI2MOD I generated a
>> PVPT QUAD model. Then I ran the model in QUAD connected to the same
>> pullup resistor I had used to generate the HSPICE data with, connected
>> directly to the buffer. The two wave forms were different, by a lot.
>> The two solutions I came up with were
>>
>> 1.) Take the Time & voltage data generated from the HSPICE run and adjust
>> the time zero to be right at the time when the output buffer starts
>> turning on. As opposed to when SPICE time zero started, which is on
the
>> input side of the buffer with a PWL model.
>>
>> 2.) Use the 10290 option when generating a model. This seemed to be a more
>> accurate model, and didn't require any data manipulation.
>>
>> Any comments?
>>
>> Mark Nass
>>
>
>
>