From: Mark Alexander ([email protected])
Date: Mon Apr 30 2001 - 10:36:33 PDT
Larry,
On your 3.125 link, what level of pre-emphasis are
you using? 15%? More? Less?
Thanks,
mark
Larry Miller wrote:
> 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 - 10:11:47 PDT