Re: [SI-LIST] : How to model effect of vias on nearby traces?

About this list Date view Thread view Subject view Author view

From: Jan De Geest (jan.degeest@wanadoo.be)
Date: Thu Mar 28 1991 - 12:47:52 PST


Ron,

This Agilent tool you were mentionning, does it contain a library of
parameterized models (with the parameters being the pad size, antipad size,
hole diameter, etc.), something like the circuit models in ADS ? Or does one
need to draw the whole geometry like in some of the full-wave 3d tools
(Ansoft, Zeland, ..), which can take a very long time to do so. What is the
name of this tool ?

Jan De Geest.

-----Oorspronkelijk bericht-----
Van: Ron Miller <rmiller@brocade.com>
Aan: 'Aubrey_Sparkman@Dell.com' <Aubrey_Sparkman@Dell.com>; jian@zeland.com
<jian@zeland.com>; bpatel@cyras.com <bpatel@cyras.com>;
ldmiller@rhapsodynetworks.com <ldmiller@rhapsodynetworks.com>;
mgreim@sonusnet.com <mgreim@sonusnet.com>; si-list@silab.eng.sun.com
<si-list@silab.eng.sun.com>
Datum: dimanche 25 mars 2001 21:49
Onderwerp: RE: [SI-LIST] : How to model effect of vias on nearby traces?

>Agilent also has tools for modeling vias and traces in the
>ADS and MDS suites which I believe to be the most accurate of
>all the simulation tools for passive structures. The models
>for vias are, via, pad, antipad and you build a stackup of these
>elements for a multi-layer board.
>
>Then according to which layer has the source and the load, it
>simulates in the frequency domain the effects of the stubs, the
>thru section of the via an the capacitance to the ground/power
>layer antipads.
>
>Ron Miller
>
>-----Original Message-----
>From: Aubrey_Sparkman@Dell.com [mailto:Aubrey_Sparkman@Dell.com]
>Sent: Friday, March 23, 2001 7:56 AM
>To: jian@zeland.com; bpatel@cyras.com; ldmiller@rhapsodynetworks.com;
>mgreim@sonusnet.com; si-list@silab.eng.sun.com
>Subject: RE: [SI-LIST] : How to model effect of vias on nearby traces?
>
>
>Bhavesh,
>In addition to IE3D from Zeland, there are also 3d tools from Ansoft.
>Probably there are other tools as well. But if you can follow good layout
>practices, you probably don't need to worry. BTW, I would caution against
>putting a via in between your differential pair.
>
>Good luck!
>Aubrey Sparkman
>Signal Integrity
>Aubrey_Sparkman@Dell.com
>(512) 723-3592
>
>
>> -----Original Message-----
>> From: Jian X. Zheng [mailto:jian@zeland.com]
>> Sent: Thursday, March 22, 2001 8:05 PM
>> To: Patel, Bhavesh; Aubrey_Sparkman@exchange.dell.com;
>> ldmiller@rhapsodynetworks.com; mgreim@sonusnet.com;
>> si-list@silab.eng.sun.com
>> Subject: RE: [SI-LIST] : How to model effect of vias on nearby traces?
>>
>>
>> Hi, Mr. Patel:
>>
>> Please try our IE3D full wave electromagnetic simulator. It
>> is perfect for
>> the structure you want to analyze. Please do not consider full wave
>> simulators are difficult to use. The IE3D takes seconds or
>> minutes to solve
>> your problem accurately. Our MDSPICE simulator can extract
>> wide band SPICE
>> model from the s-paramters generated from IE3D and it can
>> even perform a
>> time domain simulation on the s-parameters for your long interconnect
>> structures.
>>
>> Best regards,
>>
>> --------------------------------------------------------------
>> ---------
>> Jian-X. Zheng, Ph.D
>> Zeland Software, Inc., 48890 Milmont Drive, 105D, Fremont, CA
>> 94538, U.S.A.
>> Tel: 510-623-7162, Fax: 510-623-7135, Web: http://www.zeland.com
>> ---------------------------------------------------------------------
>> Special Announcements: (1) IE3D 8.0 is released. The IE3D 8.0 has
>> implementation of boxed Green's functions, periodic Green's
>> functions, and
>> advanced iterative matrix solvers for large structures. Using the AIMS
>> matrix solvers, you will be able to solve large RF IC and
>> antenna array
>> problems. An example of an 8 by 8 antenna array takes less
>> than 100 MB RAM
>> to solve on the AIMS III matrix solver. (2) The s-parameter
>> SPICE simulator
>> MDSPICE 2.1 is released. The MDSPICE 2.1 has a robust time
>> domain engine
>> accepting s-parameters from full wave simulators. Its time
>> domain simulation
>> normally can guarantee the causality conditions for lossy
>> transmission lines
>> longer than 1 foot. The MDSPICE 2.1 also features wide band
>> SPICE model
>> extraction, eye pattern display and non-linear modeling for
>> both digital and
>> analog circuits. (3) The FIDELITY 3.0 is formally released.
>> It has many good
>> features to enhance 3D modeling in wireless communications.
>> --------------------------------------------------------------
>> --------------
>> --
>>
>> > -----Original Message-----
>> > From: owner-si-list@silab.eng.sun.com
>> > [mailto:owner-si-list@silab.eng.sun.com]On Behalf Of Patel, Bhavesh
>> > Sent: Thursday, March 22, 2001 5:18 PM
>> > To: 'Aubrey_Sparkman@Dell.com'; ldmiller@rhapsodynetworks.com;
>> > mgreim@sonusnet.com; si-list@silab.eng.sun.com
>> > Subject: RE: [SI-LIST] : How to model effect of vias on
>> nearby traces?
>> >
>> >
>> > Hi! I agree with Aubrey that no SPICE tool can look at the effect
>> > of cahnge
>> > in impedance when the trace is routed adjacent to an anti-pad or
>> > via because
>> > I tried playing with Specctraquest which gives you the
>> parasitics of a
>> > segment of a trace and the impedance remained the same when I
>> > moved the via
>> > away.
>> > Do you know which field solver can look at this issue?
>> Because I wanted to
>> > see if I route a differential high speed trace around multiple
>> > vias(forms a
>> > hexagon when it encounters a via)if ther is any impedance change.
>> > Thanks
>> > Bhavesh
>> >
>> > -----Original Message-----
>> > From: Aubrey_Sparkman@Dell.com [mailto:Aubrey_Sparkman@Dell.com]
>> > Sent: Thursday, March 22, 2001 4:19 PM
>> > To: ldmiller@rhapsodynetworks.com; mgreim@sonusnet.com;
>> Patel, Bhavesh;
>> > si-list@silab.eng.sun.com
>> > Subject: RE: [SI-LIST] : How to model effect of vias on
>> nearby traces?
>> >
>> >
>> > Larry and Michael,
>> > Can we agree that a trace through any pin field will see
>> either no change,
>> > higher impedance, or lower impedance, all depending on the design
>> > of the pad
>> > stack, trace width, and stackup?
>> >
>> > Bhavesh,
>> > I would answer that no SPICE including HSpice can determine the
>> > impedance of
>> > a trace as it passes through a pin field. For that you
>> need another tool.
>> > To understand the effects of a trace going through a pin
>> field, you need a
>> > two step process. I think that all would agree that since these
>> > effects are
>> > geometry (trace width and pad stack design) and material
>> > specific, you would
>> > need either a TDR (after design) or a Field Solver to determine the
>> > impedance of the trace as it passes through the pin field.
>> >
>> > Only after you determine those impedances can you use your
>> > favorite SPICE to
>> > determine the effect of those impedances on your signal. Of
>> > course, if your
>> > board is already designed and assembled, you can use a TDR
>> > without SPICE to
>> > look at those reflections.
>> >
>> > Aubrey Sparkman
>> > Signal Integrity
>> > Aubrey_Sparkman@Dell.com
>> > (512) 723-3592
>> >
>> >
>> > > -----Original Message-----
>> > > From: Larry Miller [mailto:ldmiller@rhapsodynetworks.com]
>> > > Sent: Thursday, March 22, 2001 4:50 PM
>> > > To: 'Greim, Michael'; Larry Miller; 'Patel, Bhavesh';
>> SI_LIST (E-mail)
>> > > Subject: RE: [SI-LIST] : How to model effect of vias on
>> nearby traces?
>> > >
>> > >
>> > > Let's say for argument that a trace runs directly over
>> the center of a
>> > > circular antipad area on the reference plane, and the antipad
>> > > diameter is
>> > > larger than the trace width.
>> > >
>> > > Yes, there is no reference under the trace, but wouldn't the
>> > > return paths of
>> > > least inductance go around the rims of the circular antipad?
>> > > That is not a
>> > > much longer path length unless the antipad is huge, so maybe
>> > > that is why
>> > > there does not seem to be much effect.
>> > >
>> > > What seems to really affect things is where you have a gap
>> > > such that the
>> > > return currents have to seek a much longer path length.
>> > >
>> > > Hmmm?
>> > >
>> > > Larry Miller
>> > >
>> > > -----Original Message-----
>> > > From: Greim, Michael [mailto:mgreim@sonusnet.com]
>> > > Sent: Thursday, March 22, 2001 2:40 PM
>> > > To: 'Larry Miller'; 'Patel, Bhavesh'; SI_LIST (E-mail)
>> > > Subject: RE: [SI-LIST] : How to model effect of vias on
>> nearby traces?
>> > >
>> > >
>> > > Wouldn't part of the effect (perhaps a more significant
>> > > part) be how big the antipad is on the reference plane and
>> > > whether the signal in questions is routed over it or not?
>> > > I have seen some antipad requirements so large that a trace
>> > > could be routed over a wafer thin piece of plane to the
>> > > point that the trace is essentially routed over no reference
>> > > at all.
>> > >
>> > > Comments?
>> > >
>> > > Best Regards,
>> > >
>> > > Michael C. Greim Sonus Networks
>> > > mgreim@sonusnet.com 978-589-8336
>> > >
>> > > Making the world safe for digital signals everywhere
>> > >
>> > > And all this science I don't understand
>> > > It's just my job six days a week
>> > >
>> > > The time is gone. The email's over
>> > > Thought I'd something more to say......
>> > >
>> > >
>> > > -----Original Message-----
>> > > From: Larry Miller [mailto:ldmiller@rhapsodynetworks.com]
>> > > Sent: Thursday, March 22, 2001 4:42 PM
>> > > To: 'Patel, Bhavesh'; SI_LIST (E-mail)
>> > > Subject: RE: [SI-LIST] : How to model effect of vias on
>> nearby traces?
>> > >
>> > >
>> > > I have seen some high speed connector TDR plots where traces
>> > > are routed
>> > > through pin fields on back/midplanes. This is similar to
>> > > passing near a via,
>> > > even worse I would think. I have also done TDR's on our
>> own boards.
>> > >
>> > > The effect seems to be very small (a few % of 50 ohms) and of
>> > > short duration
>> > > in time, which of course corresponds to very high frequencies
>> > > (10's of GHz).
>> > >
>> > > One view.
>> > >
>> > > Larry Miller
>> > >
>> > > -----Original Message-----
>> > > From: Patel, Bhavesh [mailto:bpatel@cyras.com]
>> > > Sent: Wednesday, March 21, 2001 8:06 PM
>> > > To: SI_LIST (E-mail)
>> > > Subject: [SI-LIST] : How to model effect of vias on nearby traces?
>> > >
>> > >
>> > > Hi! I wanted to know how do I simulate the effect on the
>> impedance..
>> > > reflection on a trace/signal when it is very close to a via.
>> > > It does not go
>> > > thru the via but passes very close to it. Can I model this in
>> > > HSPICE? And if
>> > > yes how/
>> > > Thanks in advance
>> > > Bhavesh
>> > >
>> > > **** To unsubscribe from si-list or si-list-digest: send e-mail to
>> > > majordomo@silab.eng.sun.com. In the BODY of message put:
>> UNSUBSCRIBE
>> > > si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
>> > > si-list archives are accessible at http://www.qsl.net/wb6tpu
>> > > ****
>> > >
>> > > **** To unsubscribe from si-list or si-list-digest: send e-mail to
>> > > majordomo@silab.eng.sun.com. In the BODY of message put:
>> UNSUBSCRIBE
>> > > si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
>> > > si-list archives are accessible at http://www.qsl.net/wb6tpu
>> > > ****
>> > >
>> > > **** To unsubscribe from si-list or si-list-digest: send e-mail to
>> > > majordomo@silab.eng.sun.com. In the BODY of message put:
>> UNSUBSCRIBE
>> > > si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
>> > > si-list archives are accessible at http://www.qsl.net/wb6tpu
>> > > ****
>> > >
>> > >
>> >
>> >
>> > **** To unsubscribe from si-list or si-list-digest: send e-mail to
>> > majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE
>> > si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
>> > si-list archives are accessible at http://www.qsl.net/wb6tpu
>> > ****
>> >
>>
>>
>
>
>**** To unsubscribe from si-list or si-list-digest: send e-mail to
>majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE
>si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
>si-list archives are accessible at http://www.qsl.net/wb6tpu
>****
>
>

**** To unsubscribe from si-list or si-list-digest: send e-mail to
majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu
****


About this list Date view Thread view Subject view Author view

This archive was generated by hypermail 2b29 : Thu Jun 21 2001 - 10:11:20 PDT