From: Larry Miller ([email protected])
Date: Mon Apr 30 2001 - 07:19:49 PDT
In our case (a back plane) we had striplines throughout the thickness of the
board (multiple routing layers). The board is nearly 0.25" thick. We did the
unused pad removal, as suggested here by others, and we also followed the
AMP design rules for pad size and antipad (annulus) diameter. If you do
that, you get very even characteristics. Yes, there is a short capacitance
dip in a TDR, but it is so short as to correspond to a very high frequency
or shorter rise time-- higher than we would be interested in.
We got the pitch on counter boring from the back and also on using blind
vias from some PCB vendors. We decided to try it without, since the papers I
have seen on these topics seem to deal with miniscule effects unless you are
up in the 10GHz zone, which we were not. I would not argue with anyone who
said they wanted to do these things.
Since this thread started, I have had the opportunity to look closely at the
board and plug in test boards both with an HP 8753 VNA and a TEK CSA8000
scope with TDR plug in. Yes, you can see the bobbles in the VNA sweep caused
by the pin vias. You can also see the small (<10%) impedance discontinuities
at the connectors. The impedance effects caused by routing through the HS-3
pin fields in the AMP-recommended manner were miniscule (<0.5%), which I was
very happy with.
Furthermore, we have used some SERDES eval boards to actually send 3.125 GHz
8B/10B PRBS (random data) signals through the backplane. All is well. Good
eye opening (pre-emphasis required!) on 20-24" paths through 2 connectors.
Very little added jitter, relative to the SERDES outputs, which are in turn
comparable to the oscillator jitter. Plenty good for our purposes.
Larry Miller
-----Original Message-----
From: [email protected] [mailto:[email protected]]
Sent: Monday, April 30, 2001 3:56 AM
To: [email protected]; [email protected];
[email protected]
Subject: Re: [SI-LIST] : RE: 2.5 GHz in FR4
Larry,
After reading all of the replies to the 2.5GHz questiion, I can see the need
for using stripline to keep phaseshift constant on long runs. In trying to
make the stubs a part of the transmission line, wouldn't it be advisable to
utilise most of the via as part of the line by using the stripline located
on
the opposite side of a card from the IC?
Consider the 8 layer stackup shown here for clarification.
------- Sig and IC layer
------------- Plane
------- Sig
------------- Plane
------------- Plane
------- Sig 2.5 GHz stripline
------------- Plane
------ Sig
The stub resulting from the the unused portion of the via is reduced in
length. The trick would be to make the vias look like the transmission line
impedance.
Another thought--It seems like an imbedded microstrip line would possess
almost the same qualities of a stripline in terms of dielectric affecting
phaseshift. Can a card be made so that the vias would go only from the IC
layer to an imbedded microstrip layer directly below? This would get rid of
any stubs. What do you think?
Richard Ellison
972-569-8317
**** To unsubscribe from si-list or si-list-digest: send e-mail to
[email protected]. 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
****
This archive was generated by hypermail 2b29 : Thu Jun 21 2001 - 10:11:46 PDT