From: Ritchey Lee ([email protected])
Date: Tue Feb 13 2001 - 05:41:36 PST
I've built actual test PCBs to allow the measurement of this. Yes, the
impedance drops, but that is the main problem.
Lee
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 <[email protected]> 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
> > > > > >[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
> > > > > >****
> > > >
> > > >
> > > > **** 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
> > > > ****
> > > >
> > >
> > > __________________________________________________
> > > 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
> > > [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
> > > ****
> >
> > **** 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
> > ****
>
> ------------------------------------------------------------------------
> [Image]
>
> Perry Qu <[email protected]>
> Signal Integrity Specialist
> Alcatel CID
> Product Integrity
>
> Perry Qu
> Signal Integrity Specialist <[email protected]>
> Alcatel CID
> Product Integrity
> 600 March Road Work: (613)7846720
> Kanata
> ON
> K2K 2E6
> Canada
> Additional Information:
> Last Name Qu
> First Name Perry
> Version 2.1
**** 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 : Tue May 08 2001 - 14:30:50 PDT