**From:** Dima Smolyansky (*dima@tdasystems.com*)

**Date:** Wed Jul 19 2000 - 10:17:35 PDT

**Next message:**Greg Erker: "[SI-LIST] : Split planes for DACs?"**Previous message:**Muranyi, Arpad: "[SI-LIST] : TDR-ing a via"**In reply to:**Muranyi, Arpad: "[SI-LIST] : TDR-ing a via"

RE: [SI-LIST] : inductance extracted by ansoft SI3DArpad:

Of course, one could not have a "T" split in the TDR path, that confuses the measurement and the user.

However, if you have a pad and a (very) short trace leading to the via, and then a de-embedding structure which is the same size pad and trace but no via, you could TDR both, and the integral of the difference will give you the capacitance of the via. This is documented in JEDEC standard I mentioned, as well as in the recent IBIS Accuracy Handbook. This computation is also automated in our TDR software tools.

Again, you can't have a "T" split when doing a TDR, but if you run into multiple reflections when TDR'ing a complex multisegment structure, you can de-embed the multiple reflections and get the true impedance profile using the impedance deconvolution algorithm, reported many times by different authors. This algorithm gives you accurate impedance readouts at each point in the TDR trace, and is also implemented in our TDR software tools.

Thanks,

===================

Dima Smolyansky

TDA Systems, Inc.

11140 SW Barbur Blvd., Suite 100

Portland, OR 97219

(503) 246-2272

(503) 246-2282 (fax)

(503) 804-7171 (mobile)

http://www.tdasystems.com

The Interconnect Modeling Company(TM)

----- Original Message -----

From: Muranyi, Arpad

To: si-list

Sent: Wednesday, July 19, 2000 9:43 AM

Subject: [SI-LIST] : TDR-ing a via

Dima,

Thanks for your response. I was writing about the situation when the via

is probed with some PCB trace between it and the TDR probe's end, but I

see how your suggestion can yield better results.

However, I have a question about the technique you described. If I put

the TDR probe directly on the via which has traces going away from both

of its ends, I will get multiple reflections. Is that not going to mess

up and invalidate my TDR measurement? It sounds to me that your method

could only be applied to a specially fabricated test fixture where the

via stands almost alone by itself.

Arpad

==========================================================================

-----Original Message-----

From: Dima Smolyansky [mailto:dima@tdasystems.com]

Sent: Monday, July 17, 2000 3:18 PM

To: si-list

Subject: Re: [SI-LIST] : inductance extracted by ansoft SI3D

Dear Arpad:

Actually, if you look at the JEDEC standard for package characterization from TDR which I mentioned early in this discussion, it assumes that you can contact your via either directly with a microwave probe or through a closely located pad. That way the losses, in what essentially is a test fixture for your via, are not influencing the measurement.

Of course, if your via is too small to be seen with a TDR, you can chain a couple of them together or use other techniques to get better accuracy.

As far as modeling losses with TDR, you can get the S-parameter data computed from TDR relatively easily, using, for example, our IConnect TDR software. If you have a network analyzer, of course, you have no need for such computation.

Thanks,

===================

Dima Smolyansky

TDA Systems, Inc.

11140 SW Barbur Blvd., Suite 100

Portland, OR 97219

(503) 246-2272

(503) 246-2282 (fax)

(503) 804-7171 (mobile)

http://www.tdasystems.com

The Interconnect Modeling Company(TM)

----- Original Message -----

From: Muranyi, Arpad

To: si-list

Sent: Monday, July 17, 2000 2:22 PM

Subject: RE: [SI-LIST] : inductance extracted by ansoft SI3D

There is one thing that doesn't get mentioned in this discussion.

Even if your TDR head is capable of 35 ps, which corresponds to

something between 1-2 mm, the problem is that by the time this

signal from the TDR head gets to the via of interest, the rise

time will be much less due to losses and dispersion in the path

to the via. So chances are that you may not see it at all...

Another thing I would like to mention is that I am not aware of

any techniques that can give you the loss parameters from a TDR

measurement. Transmission line models can't be modeled without

the losses accurately any more.

Arpad Muranyi

Intel Corporation

================================================================

-----Original Message-----

From: Dima Smolyansky [mailto:dima@tdasystems.com]

Sent: Monday, July 17, 2000 11:45 AM

To: si-list

Subject: Re: [SI-LIST] : inductance extracted by ansoft SI3D

Matt:

TDR's typical resolution is, in fact 1-2mm, assuming reflected rise time of 25-40ps. If you try and TDR your tiny package via, you probably will see a very small blip (dip?), which you could probably correlate to some capacitive / inductive value, but with moderate accuracy.

However, if a 35 ps TDR does not see an element, one probably needs to ask him/herself a question: What is the rise times of the actual signals propagating through that package, and will these signals see this tiny discontinuity? As you know, for slower rise times, the capacitive/inductive discontinuities become even less visible to the signals propagating through it, and if your driver rise time is 100ps, you won't see the tiny via at all.

Thanks,

===================

Dima Smolyansky

TDA Systems, Inc.

11140 SW Barbur Blvd., Suite 100

Portland, OR 97219

(503) 246-2272

(503) 246-2282 (fax)

(503) 804-7171 (mobile)

http://www.tdasystems.com

The Interconnect Modeling Company(TM)

----- Original Message -----

From: Matt Kaufmann

To: si-list

Sent: Monday, July 17, 2000 10:12 AM

Subject: RE: [SI-LIST] : inductance extracted by ansoft SI3D

Does TDR have enough resolution to isolate the effects of a single package via (maybe only 0.1-0.3mm long) from other elements (traces, other vias) in the package? My understanding is that TDR resolution is on the order of 1-2 mm (after converting time to distance).

Matt

-----Original Message-----

From: owner-si-list@silab.eng.sun.com [mailto:owner-si-list@silab.eng.sun.com]On Behalf Of Dima Smolyansky

Sent: Monday, July 17, 2000 9:35 AM

To: si-list

Subject: Re: [SI-LIST] : inductance extracted by ansoft SI3D

Hello:

There is always, of course, the way of the TDR.

If the via is so long compared to system rise time that it needs to be considered a distributed elements, TDR extracts the Z and Td quite nicely.

If it is necessary to compute L and C of the via separately, extending the JEDEC publication JEP-123 from packages to other elements, one can do it, as long as one is able to create appropriate test structures beforehand. R is a separate issue, but R is typically a small number, millohm one hopes, is it not? In that case, it is best measured with a DC meter, which can provide an accurate value.

There are also TDR techniques for computing partial or loop inductance values, depending which is required.

Thanks,

Dima Smolyansky

TDA Systems, Inc.

11140 SW Barbur Blvd., Suite 100

Portland, OR 97219

(503) 246-2272

(503) 246-2282 (fax)

(503) 804-7171 (mobile)

http://www.tdasystems.com

The Interconnect Modeling Company(TM)

----- Original Message -----

From: Hassan Ali

To: si-list

Sent: Monday, July 17, 2000 7:47 AM

Subject: RE: [SI-LIST] : inductance extracted by ansoft SI3D

* > > 2.For a via through several power and ground planes, does the SI 3D
*

* > > consider the effects of those planes when doing the extraction?
*

* > >
*

* >
*

* > For this I believe you need a full wave solver such as their HFSS. Edge
*

* > rate (frequency content) & geometry really are the factors. If you edge
*

* > rate is slow compared to the geometry, then the complication of an
*

* > additional solver MAY not be necessary. But, since we MAY not know all
*

* > those rules of thumb & guidelines, take no chances & use a full wave because
*

* > you probably do have edge rates which are "fast". Your investment in
*

* > understanding a refined full wave solver will be worth it.
*

As to the original question, AFAIK (as far as I know) Ansoft SI Q3D is NOT capable of computing via parasitics in consideration to individual planes. You see, SI Q3D considers the entire via structure comprising of the signal traces connected to the via, the via barrel (the plating on the via hole), and all the pads at different layers, as ONE conductor. ALL the ground planes are considered connected hence they make ONE conductor. In that case, the self L and R values computed for the via structure are for the ENTIRE via structure as mentioned above (i.e. not just for the via barrel), and the capacitance to ground is with reference to ALL the ground planes (i.e. you don't get separate values for capacitance with reference to EACH individual ground plane). That information is not very useful for critical SI analysis. And unfortunately, I don't know of any software tool that can accurately compute separate parasitics. Any suggestions?

To illustrate further the problem in question, suppose I want to include via parasitics for a signal that goes from the top pcb layer to an inner signal layer, then I need to include via parasitics of only that portion of the via that gets into the path of my signal i.e. not the parasitics of the entire via structure. Any body knows how to do that with the presently available tools?

As to the capabilities of HFSS, I think many people make wrong assumptions on how full-wave field solvers can help us (SI engineers). First of all HFSS would NOT spit out via parasitics! Using your various signal traces as "ports", HFSS can accurately compute scattering (S) parameter matrix for all the ports. These S-parameters are computed for each propagation mode of interest (e.g. TEM mode) and indeed takes into account the electromagnetic (EM) field interactions of all the structures in the geometry of the problem (e.g. for a via, all the conductors, power and ground planes).

That is well and good, but the problem is that you CANNOT (easily) separate individual interactions in terms of R, L, and C parasitics. The only method I know of is to find a lumped-element equivalent circuit (which may not be unique) and use a microwave circuit simulator (like Touchstone, Libra, ADS, MDS, Ensemble, SuperCompact, APLAC, etc.) to optimize the R, L, and C, values to make the equivalent circuit have the same S-parameters as the original 3D structure. This is a painful process and at best not accurate and reliable. This is because, at high frequencies, all the parasitics are distributed and therefore cannot (easily) have an accurate lumped-element equivalent. Am I too much of a pessimist here? Any ideas of what works best?

Regards.

Hassan.

**** 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

****

**Next message:**Greg Erker: "[SI-LIST] : Split planes for DACs?"**Previous message:**Muranyi, Arpad: "[SI-LIST] : TDR-ing a via"**In reply to:**Muranyi, Arpad: "[SI-LIST] : TDR-ing a via"

*
This archive was generated by hypermail 2b29
: Wed Nov 22 2000 - 10:50:49 PST
*