[SI-LIST] Re: local and global ground
- From: Larry Smith <ldsmith@xxxxxxxxxxxxxxxxxx>
- To: si-list@xxxxxxxxxxxxx
- Date: Tue, 29 Jan 2002 08:24:31 -0800 (PST)
This is a very interesting discussion. I often use power plane
transmission line models that completely account for all current into
and out of a driver or receiver. The power path is very low impedance
for loop current but very high impedance to current that does not
return in the power path ...kind of like our products. :)
If there happens to be a sneak path to spice node zero, very strange
simulation occurs. The circuit can fail to converge or else very
unrealistic voltages are obtained, sometimes 1000's of volts if current
sources are involved. This happens when driver or receiver circuits
force current to spice node 0 instead of allowing it to return through
the power terminals of the circuit.
An easy way to check for this is to put an ammeter (zero volt voltage
source) on all ports of the circuit. Sum the currents through the
ammeters in an output parameter. Kirkoff tells us that the sum should
be zero. If it is not, you have a sneak path to spice node zero. That
is like current jumping from somewhere inside of our product to the
center of the earth without ever going through our packaging. Hmmmm.
This can happen even if there are no global or specific references to
spice node zero in the circuit. Many transistor .model statements
manage to "eat" the current. These models will cause havoc in power
distribution analysis where all current is expected to return through
the packaging.
regards,
Larry Smith
Sun Microsystems
> Delivered-To: si-list@xxxxxxxxxxxxx
> Date: Tue, 29 Jan 2002 10:37:19 -0500
> From: "Perry Qu" <perry.qu@xxxxxxxxxxx>
> X-Accept-Language: en
> MIME-Version: 1.0
> To: si-list <si-list@xxxxxxxxxxxxx>
> Subject: [SI-LIST] Re: local and global ground
> Content-Transfer-Encoding: 8bit
> X-archive-position: 1859
> X-listar-version: Listar v1.0.0
> X-original-sender: perry.qu@xxxxxxxxxxx
> X-list: si-list
>
>
> Andy:
>
> Thank you for sharing your experience on this. I rechecked the 2 models from
> 2 vendors. I did not find any .Global statements in either of them. But in
> one of the model, I do find node 0 inside the model, which may be the reason
> that give me "inductor/voltage loop" error.
>
> In the case of the second model, there is no 0 node inside the model and the
> vendor claim that they run this type of simulation without any problem in
> another SPICE tool. I have sent the HSPICE deck to the vendor and ask them
> to try it out. This is case where I see big spike on ground (amplitude even
> a few times bigger than my incident voltage swing).
>
> Regards
>
> Perry
>
> "Ingraham, Andrew" wrote:
>
> > I have done what you are trying to do ... use a local non-ground
> > reference in HSPICE ... and it can work if done right.
> >
> > Sometimes you run into problems where some vendor's model has hidden
> > connections to ground, either because it is encrypted so you can't tell
> > what the heck is in it, or because they did something incredibly
> > un-user-friendly like having .GLOBAL node statements within their
> > subcircuits. I have spent hours un-doing this kind of junk in vendor
> > models.
> >
> > But in your case the daughter card side is so simple, that I suspect the
> > connector models are at fault.
> >
> > Are you sure the connector models were created to include what one might
> > call "common mode" effects, when the two sides are unhinged? If it only
> > models local effects between neighboring pins, or if it was intended to
> > have reference node 0 on both sides, it might have completely missed the
> > effects between the two boards. Getting a totally "correct" model that
> > really behaves just like the real connector, under all conditions, isn't
> > something that just automatically pops out of the modeling process.
> > Just like SPICE's transmission line model ignores the common-mode
> > (unless we explicitly include it, which takes some effort), the
> > connector models might have done the same.
> >
> > What you are seeing is probably not "numerical noise", but rather "real"
> > noise from the point of view of the simulator, but due to poor modeling.
> > There's a difference.
> >
> > I am puzzled why the second vendor's model gives you an
> > "inductor/voltage loop" error message, which is fixed by connecting the
> > daughter card side to node 0. Usually that error means there is a
> > connection that shouldn't be there, like maybe you unintentionally
> > re-used a node number. I might have expected a "floating node" or "no
> > DC path to ground" error message, in your case. Track down exactly
> > where that inductor/voltage loop is, it might tell you something.
> >
> > Andy
> >
> > ------------------------------------------------------------------
> > 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 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
> >
>
> --
> Perry Qu
>
> Product Integrity | 600 March Road
> Alcatel Canada | Ottawa, ON K2K 2E6, Canada
>
> DID: (613) 7846720 | FAX: (613) 5993642
>
>
> ------------------------------------------------------------------
> 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 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 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:
