Subject:                              Time:  10:02 AM
  OFFICE MEMO         RE>RE>Ground Planes                   Date:  2/12/96

Kitty

In your inquiry, you have several good questions that is too long to cover
through technet.  If you want, I'll be glad to provide you with additional
information if you need/request it.  The following are brief responses to your
inquiries.

*  Information on ground planes, some of the best information on printed board
power/ground planes is contained in the EMC (electromagnetic compatability)
world.  Some of the good texts and info are available, the one's I'm most
familiar with are from Don White consultants, he had two companies,
Interference Control Technologies, and Don White Consultants, Inc. (as
subsidary), they were located in  Gainsville, VA.  They have a couple of texts
with a focus on printed boards.

*  "Thin" power/ground planes can result in poor/inadequate voltage drops in
the power/ground distribution system, especially for the low frequency direct
current (dc) voltages.  As a rule-of-thumb, the sheet resistance of 70
micrometer (2 oz/sq.ft.) Cu foil is about 300 microhms/sq., 35 micrometer Cu
foil is about 600 microhms/square, each halving in thickness doubles the
resistance.  Long aspect ratios (length/width) of conductors significantly
increases resistance and inductance.  Like resistors and inductors in series,
the add up, in the wrong direction toward poorer circuit performance.  When
power/ground planes are "perforated" with holes for vias, access, and
component holes, the inductance of the plane(s) increases and the distributed
capacitance decreases, the result being the power/ground plane impedance
increases, which leads to more noise in the voltage/grounding system.  End
result - most probably reduces (like guaranteed) electrical signal integrity
(including dc signals).

*  Very thin areas that separates half the board from the other half, and add
vias to increase contact.  Assuming the planes are at the same potential and
are "superimposed" additional vias between the planes may/may not help out. 
Simply stated, it depends on the number and location of the additional vias. 
In your particular application, additional vias may change the direction of
electrical current flow due to the impedances of each the planes you want to
interconnect and the quantity and location of added vias.  You must perform an
analysis over the complete range of frequencies of operation, from dc-to-the
highest ac frequency.  This is because the conductive patterns (including
power/ground planes) will form complex electrical networks that will have
various local electrical resonances between various vias.  These electrical
resonances will inject electrical signals (voltage and currents) into the
circuit with possibly undesirable results.

As mentioned in the intro. paragraph, please feel free to contact me if you
need/desire more information.

Ralph Hersey
Lawrence Livermore National Laboratory
e-mail
Phn:  510.422.7430
FAX:  510.424.6886


-------------Original Inquiry Follows ------------------
I am looking for any information regarding ground planes.
Are there any standards as to how thin the plane can be
as it gets routed throughout the board?  If you have a very thin area that
seperates half the board from the other half, does this cause 
problems?  Would it be better to add vias to increase contact?