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

About this list Date view Thread view Subject view Author view

From: Perry Qu (perry.qu@alcatel.com)
Date: Mon Mar 26 2001 - 06:51:47 PST


Hi! Ron:

Are you talking about HP Momentum for the via simulation ? Right now I'm
looking into the HP Picosecond Interconnect Suite. As I understand, this tool
consists of several modules. I was a bit confused about the difference between
this Suite and ADS/MDS, the later seems to be intended for RF/digital
design. Any idea the difference between the two ?

Thanks

Perry Qu

Ron Miller wrote:

> 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