Re: [SI-LIST] : Copper balance

About this list Date view Thread view Subject view Author view

From: Ritchey Lee (leeritchey@earthlink.net)
Date: Tue Feb 13 2001 - 05:43:06 PST


Why would you have very high EM field concentrations?

Lee

DORIN OPREA wrote:

> Hi,
>
> Thank you very much for your comments. This copper balance, as I see it in our
> case , is not an issue from signal integrity point of view (we make sure that
> no signals are routed in these areas). My main worry is the possible resonance
> on this floating copper one may have when a card with this construction works
> within a system with very high EM field concentration.
>
> Thanks,
> Dorin
>
> Perry Qu wrote:
>
> > Hi! Richey:
> >
> > Thank you for your comments. I did some simulation recently using a 3D field
> > solver to calculate how the isolated copper dots affect the transmission
> > line. My original intention is not to study the copper dots due to copper
> > balance, but to study how embedded microstrip lines are affected by copper
> > pads on the components side. e.g., I saw many routing done in a way similar
> > to the cases shown in the attached jpg file, where you have repeated copper
> > pads right on top of a embeded-microstrip line.
> >
> > From the simulation, I find that the copper dots will increase the
> > capacitance of the transmission line while the inductance does not change
> > much. This results in lower impedance as you mentioned in your comments. In
> > my particular simulation, the impedance is about 6% lower for transmission
> > line with copper dots.
> >
> > Regards
> >
> > Perry Qu
> >
> > Ritchey Lee wrote:
> >
> > > These bits of copper don't function as antennas. If there are many of
> > > them close to controlled impedance traces, they will lower the
> > > impedance. That's the primary concern. It is pretty easy to simulate
> > > their effect with a 2D field solver. That's much better than some
> > > arbitrary "20H" or other rule. What one does is analyse how near copper
> > > in the same layer or adjacent layers lower impedance. Then, it is a
> > > matter of moving the copper away and seeing when the effect on impedance
> > > is tolerable.
> > >
> > > What one learns when this is done is that this kind of fill on an
> > > adjacent layer when it lies over the top of a trace has a noticable
> > > effect on impedance. When this fill is on the same layer, it has no
> > > more effect than adjacent traces. So, on same layer, the spacing that
> > > is acceptable for near traces works. On adjacent layers, no copper over
> > > a trace and back away the same spacing as for adjacent layer.
> > >
> > > Hope this helps.
> > >
> > > Lee
> > >
> > > Dave Hoover wrote:
> > >
> > > > Dorin,
> > > > (From a Fabrication Stand Point)
> > > > My experience is more around something I've heard
> > > > called the "antennae effect" where the floating
> > > > (isolated) copper will be capacitive and couple with
> > > > any signals close by. So many fabricators tend to
> > > > break the copper thieving up into small isolated
> > > > features. (circles or squares) A couple of important
> > > > things to comment on would be to maintain the
> > > > isolation of these features away from other traces or
> > > > pads. (20H Rule) And to make sure that when the
> > > > fabricator generates the thieving that they also
> > > > include ALL signals contained within each reference
> > > > plane group. (i.e., a dualstripline would need both
> > > > signals (temporarily) merged to generate the pattern.
> > > > Or if layers 1 and two were signals, they would also
> > > > need to be merged to generate the thieving or else the
> > > > squares might end up being rignt on top of a signal
> > > > trace.)
> > > >
> > > > Dave Hoover - Director of Technology
> > > >
> > > > --- DORIN OPREA <dorin.oprea@alcatel.com> wrote:
> > > > > Thanks Chris. The main problem is the PCB vendor
> > > > > wanted to have 40% copper
> > > > > convereage on the layer and this implies small
> > > > > spacing between the floating copper
> > > > > geometries. Having squares 5x5 mm with the spacing
> > > > > 10 mm will give < 25% copper
> > > > > coverage; therefore less spacing is required. But
> > > > > what is the smallest spacing and
> > > > > what is the copper geometry to get 40% ?
> > > > >
> > > > > Dorin
> > > > >
> > > > >
> > > > >
> > > > > Chris Padilla wrote:
> > > > >
> > > > > > It is called thieving and I've found so signifcant
> > > > > EMI results positive or
> > > > > > negative as a result. Just set a spacing criteria
> > > > > from any components like
> > > > > > "no closer than 500 mils to any componenet or
> > > > > trace or via or whatever."
> > > > > >
> > > > > > If the board has lots of blank space to fill, the
> > > > > EMI team may wish to
> > > > > > consider making embedded caps with the free space
> > > > > and copper flood
> > > > > > depending on the reference plane nearby. I have
> > > > > found these caps to be of
> > > > > > significant importance in controlling emissions
> > > > > and they are basically "free!"
> > > > > >
> > > > > > Good Luck----->Chris
> > > > > >
> > > > > > >Hi,
> > > > > > >
> > > > > > >I am working now on the copper balance issue we
> > > > > have on our PCBs. On the
> > > > > > >outer layer beneath the converter a copper
> > > > > surface is required (E
> > > > > > >shielding) which generates the copper balance
> > > > > issue on that particular
> > > > > > >layer and also throughout the stack up. Thus, the
> > > > > unpopulated copper
> > > > > > >space is filled with square or circle floating
> > > > > copper surfaces separated
> > > > > > >in-between. These squares are overlapping
> > > > > throughout the stack up. The
> > > > > > >question: what is the best copper geometry, its
> > > > > dimension and the
> > > > > > >spacing between these geometries ?. Copper
> > > > > balance requires as much
> > > > > > >copper as possible but EMC wants no floating
> > > > > copper and very weak
> > > > > > >coupling between noisy areas such as converter
> > > > > and any functional
> > > > > > >digital area.
> > > > > > >
> > > > > > >Your help is really appreciated,
> > > > > > >Dorin
> > > > > > >
> > > > > > >
> > > > > > >**** 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
> > > > > ****
> > > > >
> > > >
> > > > __________________________________________________
> > > > Do You Yahoo!?
> > > > Get personalized email addresses from Yahoo! Mail - only $35
> > > > a year! http://personal.mail.yahoo.com/
> > > >
> > > > **** 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
> > > ****
> >
> > ------------------------------------------------------------------------
> > [Image]

**** 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 : Tue May 08 2001 - 14:30:50 PDT