From: sweir (firstname.lastname@example.org)
Date: Thu May 11 2000 - 14:13:41 PDT
Shorting midway through a clock net sounds really bad to me. I would not
expect any reasonable decoupling measures to handle such a situation. But
something sounds a bit fishy here:
(5-10ohms) (20-40) (50)
At the transmission line side of the resistor, we should see an initial 50%
step persist for almost 2nS before the negative reflection cancels it out.
At the driver to resistor connection, we should see almost the full
amplitude of the waveform.
How do you account for the observation of 0V, and at which point was it?
In any event, for this scenario, the driver current only doubles when the
negative reflection impinges the series resistor.
It sound like something else was going on.
At 08:18 AM 5/11/00 -0700, you wrote:
>I have to disagree with your second sentence. On one board that was
>was being debugged, we found out that we were driving a clock right
>into the ground plane of our board! This resulted in a radiation
>failure of over 13 dB at a particular frequency. Upon scoping the
>clock line, we found the clock drving right around 0 V! This was only
>one line of a clock buffer (it was driving 5 or 6 other loads) that
>was series terminated. We were amazed the driver was still working
>and that the other clocks were humming along just fine. I would have
>to guess that the line was about 9 total inches long and the midway
>point marked the point of ground entry. So at least in our case, one
>single net killed us!
>At 03:46 PM, you wrote:
> >First, please be sure that your measurement is not lying to you. Things
> >have got to be really, really bad if you can reliably see your clock riding
> >on the power supply. It is very hard for a single net to do this. It is
> >more likely that all the signals triggered by that clock are contributing
> >to the problem, and / or your are getting crosstalk between your scope
> >channels due to the test set-up. So, if you only address the clock, you
> >probably won't correct your symptom as measured.
> >Even assuming that the measurement is real, and that this one clock signal
> >is the source of your troubles, I don't think your proposal is a very good
> >idea. If you successfully isolate the power pin input, the signal current
> >still has to flow through the signal trace itself through the load and back
> >through the power / ground plane structure. Isolating one end makes that
> >return path more of a problem, not less.
> >It sounds like your problem is some combination of:
> > 1. Inadequate power / ground decoupling, and
> > 2. Excessive return path inductance for the high edge rate signals.
> >Bulk capacitance is good for audio frequencies up to around 1 MHz,
> >depending on what type of capacitors you are using. It is unlikely that
> >increasing bulk capacitance will help at 64MHz.
> >On a four layer, .062 board, you are going to be hard pressed to see a
> >mounted resonant frequency on the .1 uF decoupling capacitors above 8
> >MHz. Either use enough smaller capacitors, or lots of .1's to get the
> >impedance down.
> >At 09:12 AM 5/10/00 -0400, you wrote:
> >>Hi All,
> >> I'm working on a board currently which has "high" power and ground
> >>noise. I'm looking for effective methods of reducing this noise.
> >>I spent a bit of time making power and ground noise voltage measurement on
> >>the current configuration of this board. The results show that the power
> >>and ground system have noise spikes which are 180 deg. out of phase from an
> >>output clock on the board. I won't go into the measurement set up too
> >>but here are the basics:
> >>Using two FET probes to make the measurements. The ground reference
> was the
> >>digital ground input to the board. Scope was triggered off the suspect
> >>clock (64Mhz) .
> >>I suspect that an input filter to the device generating the signal (an
> >>would improve things. I'm not sure about the correct configuration for
> >>filter. Currently there are .1uF caps across each of the input power pin.
> >>I can think of two configurations that may be effective.
> >>A ferrite bead in series with each of the input power connections (keeping
> >>the .1uF caps) may be effective but I'm not sure what "side effects" may
> >>A inductor and resistor in parallel (also keeping the .1uF caps)
> setting the
> >>values .75uH and 5 ohms.
> >>I'm not sure what the draw backs of these configurations are. Or is there
> >>are better solutions.
> >>Additionally, I plan on decreasing the power and ground spacing (the board
> >>is a four layer) to 7mils, increasing the bulk capacitance to the
> board, and
> >>possibly placing .001uF caps in parallel with each of the .1uF caps.
> >>Any comments would be appreciated
> >>Best regards
> >>David Spencer
> >>**** To unsubscribe from si-list or si-list-digest: send e-mail to
> >>email@example.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
> >firstname.lastname@example.org. 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
>email@example.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
firstname.lastname@example.org. 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 : Wed Nov 22 2000 - 10:50:17 PST