[SI-LIST] Re: Spice
- From: "Dennis Han" <Dennis.Han@xxxxxxxxxxx>
- To: <ivor@xxxxxxxxxxx>, <alan@xxxxxxxxxxxxxxxxx>
- Date: Thu, 3 Feb 2005 15:04:09 -0600
I think what you are seeing is the limitations of SPICE. Try setting the
simulation options to gear method rather than the trapezoidal method and the
transitions should look more realistic. The default options for any SPICE
simulator are generally for fast, but less accurate, simulations and haven't
changed much since the mid-80's. With today's computers (and ever 10 years
ago), slow and accurate options are still fast.
Here is an example of the options line from a HSPICE simulation that will
give the most accurate transient analysis results (unless you get a
convergence problem). I also know these options (in the correct form of
course) will work for SPICE Plus and Spectre.
* General options:
.OPTIONS ACCT=2 ACOUT=1 AUTOSTOP BADCHR CAPTAB CSHUNT=0 GSHUNT=0 DIAGNOSTIC
INGOLD=1 ITRPRT KCLTEST=1 LIMPTS=20000 LIST NODE NOPAGE OPTLST=0 OPTS
TNOM=23
* DC solution control options:
.OPTIONS ABMOS=1e-12 ABSTOL=1e-12 ABSI=1e-12 VNTOL=1e-6 ABSV=50e-6 DCCAP=1
DCFOR=5 DCSTEP=0 DV=1000 GMAX=0.1 GMINDC=1e-12 GRAMP=0 ITL1=200 ITL2=50
PIVOT=0 PIVREF=1e8 PIVREL=1e-3 PIVTOL=1e-15 RELMOS=0.05 RELTOL=1e-4
RELV=1e-4
* Pole/zero control options:
.OPTIONS CSCAL=1e12 FMAX=1e12 FSCAL=1e-6 GSCAL=1e6 ITLPZ=100 LSCAL=1e12
PZABS=1e-2 PZTOL=1e-6 RITOL=1e-6
* Transient control options:
.OPTIONS ABSVAR=0.2 CHGTOL=1e-15 CVTOL=0.2 DCAP=2 DVDT=3 EPSMIN=1e-28
EXPMAX=350 FS=0.25 FT=0.25 GENK=1 GMIN=1e-12 IMAX=100 IMIN=3.0 ITL5=0.0
KLIM=1e-2 LVLTIM=2 MAXORD=2 METHOD=GEAR MU=0.5 NEWTOL=1 RELQ=0.01
RELVAR=0.15 RMAX=2.00 RMIN=1.0e-9 TRTOL=100
I think you should use ADS, Spectre, or HSPICE. PSpice has improved but it
was not originally designed to simulate high frequencies (and hence
transmission lines). That functionality has been an afterthought in its
architecture. SPICE Plus has the same problem.
Use a product such as IFS Pro, IFS Connect, or equivalent to make your
transmission line and connector models.
Dennis
----- Original Message -----
From: "Ivor Bowden" <ivor@xxxxxxxxxxx>
To: <alan@xxxxxxxxxxxxxxxxx>
Cc: <si-list@xxxxxxxxxxxxx>
Sent: Thursday, February 03, 2005 2:20 PM
Subject: [SI-LIST] Re: Spice
> Thank you for the kind comments.
> I probed the input (after the series resistor) and output (at the
> termination resistor) of the transmission line. I thought that since I
> used a lossless line, I thought the end point should be a perfect square
> wave, delayed by the line (input & output look the same). I used a 50
> ohm 50nS transmission line. What I see is the transmission line input is
> perfect square wave, at the output the rise/fall time is slower and
> there is overshoot on both edges. If I change the generator to have some
> risetime (like in the real world) the overshoot goes away, but still the
> rise/fall time is greater than the input. Varying the terminations
> produced steps and reflections as expected.
>
> What really confused me is I set up a lossy line based on the L/C
> characteristics of a 50 ohm PCB trace. The output of that seemed clean,
> but the lossless node waveforms changed! Even when I disconnected and
> grounded the lossy line the output of the lossless line was dramatically
> changed. I think simply having a lossy line in the circuit affects the
> algorithm, but I didn't expect such a dramatic difference.
>
> I would like to model a signal source driving a short PCB trace, then
> through a connector to several feet of cable into a load, so I can see
> the results of changing the signal source circuit. The frequency isn't
> too high, rise/fall times of a few nS. I'm willing to start with
> ignoring the trace and connector for a first attempt. Do you have any
> suggestions?
>
> I have a lot to learn..
>
> Thank you,
>
> Ivor
>
> on 2/3/2005 10:15 AM Alan Hilton-Nickel wrote:
>
>>Ivor,
>>
>>I could be wrong, but I don't know of a better place to ask SPICE
>>questions. As for newbie questions, you've gone about it the right way
>>by indicating you've invested some effort before asking a pretty
>>specific question. It sounds like your simulation model is correct, at
>>least on paper, but I don't know what you mean when you say the waveform
>>isn't what you expected. You should be getting a "step" waveform, with
>>the voltage rising initially to the Vin/2 level and staying there (since
>>you're perfectly terminated). If you vary the termination at the far end
>>you should see some reflections. What waveform did you get? And where in
>>the circuit are you probing?
>>
>>Alan
>>
>>
>>Ivor Bowden wrote:
>>
>>
>>
>>>Hi SI Experts,
>>>
>>>I have finally decided to get to know Spice, after many years of circuit
>>>design work, mostly digital. To this end I downloaded the SIMetrix Intro
>>>v5.0f program, and also acquired a copy of PSPICE 9.1 Student Version. I
>>>have only worked with SIMetrix so far.
>>>
>>>I realize this is probably not the place to ask newbie questions about
>>>basic SPICE operations, so my first question is, can anyone suggest any
>>>good resources (url, list server, news group, etc) to find useful
>>>information and / or ask these types of questions? Web search finds
>>>overwhelming hits to pick through, specific recommendations are
>>>appreciated.
>>>
>>>That being asked, my next question is what is the appropriate way to
>>>model a coax cable or a PCB trace, driven by a pulse? I set up a pulse
>>>voltage source (which I assume to be "perfect", that is no source
>>>impedance), a 50 ohm series resistance to represent the source
>>>impedance, a 50 transmission line grounded on both sides of one
>>>conductor, and a 50 ohm resistor to ground at the end. But the resulting
>>>waveform was not exactly what I expected..
>>>
>>>Thanks for any comments,
>>>
>>>Ivor
>>>
>>>
>>>
>>>
>>
>>------------------------------------------------------------------
>>To unsubscribe from si-list:
>>si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
>>
>>or to administer your membership from a web page, go to:
>>//www.freelists.org/webpage/si-list
>>
>>For help:
>>si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
>>
>>List FAQ wiki page is located at:
>> http://si-list.org/wiki/wiki.pl?Si-List_FAQ
>>
>>List technical documents are available at:
>> http://www.si-list.org
>>
>>List archives are viewable at:
>> //www.freelists.org/archives/si-list
>>or at our remote archives:
>> http://groups.yahoo.com/group/si-list/messages
>>Old (prior to June 6, 2001) list archives are viewable at:
>> http://www.qsl.net/wb6tpu
>>
>>
>>
>>
>>
>>
>
>
> ------------------------------------------------------------------
> To unsubscribe from si-list:
> si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
>
> or to administer your membership from a web page, go to:
> //www.freelists.org/webpage/si-list
>
> For help:
> si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
>
> List FAQ wiki page is located at:
> http://si-list.org/wiki/wiki.pl?Si-List_FAQ
>
> List technical documents are available at:
> http://www.si-list.org
>
> List archives are viewable at:
> //www.freelists.org/archives/si-list
> or at our remote archives:
> http://groups.yahoo.com/group/si-list/messages
> Old (prior to June 6, 2001) list archives are viewable at:
> http://www.qsl.net/wb6tpu
>
>
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List FAQ wiki page is located at:
http://si-list.org/wiki/wiki.pl?Si-List_FAQ
List technical documents are available at:
http://www.si-list.org
List archives are viewable at:
//www.freelists.org/archives/si-list
or at our remote archives:
http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
Other related posts:
