I've been watching this discussion in earnest for the past ...let's just say 
it's been a long time.  My eyes have glazed over several times so I'm not 
sure if my input has been brought up before.

It is the function of both the PCB designer and the PCB fabricator to do 
everything possible to insure that the design in question is as efficient 
and reliable as possible in both fabrication and assembly.

For the designer this means that every effort should be made to understand 
the complexities of fabricating a PCB.  This information should be 
incorporated into designs in such a way as to help eliminate failure modes 
(be they in cost, yield, or on-time delivery).

The fabricator needs to perform several tasks prior to fabricating any 
product.

First, the product needs to be quoted.  This process entails collecting and 
reviewing a list of parameters which most affect the yield and on-time 
delivery (and hence price).  Theoretically speaking, the pricing process 
should occur after a Manufacturability Review has been performed.  In 
practice, board prices are agreed upon by sellers and buyers with nothing 
more than a fabrication drawing -- sometimes no even that!  The some of the 
parameters typically used in determining board pricing are number of layers, 
board size, laminate type, surface finish, gold plating requirements, and 
special stuff like buried/blind vias, buried capacitance, and 
controlled/differential impedance.  Note that the presence or lack of 
presence of non-functional pads is not in the above list.  Though presence 
of non-functional pads will change the production cost  of the product (for 
reasions outlined below) their presence is not know at this point and hence 
does not typically affect the retail selling price for the board.

Second, a Manufacturability Review needs to be performed on the design. 
 This should include a DRC (design rule check), a mechanical review of rout 
characteristics and materials, and a list of suggestions that would improve 
the yields and make the product more cost effective.  When necessary, it is 
the responsibility of the fabricator to educate the designer on fabrication 
issues that might otherwise go unnoticed.  When an  incoming part number  is 
received by Automata, a Manufacturability Review is preformed, and the 
request is almost alway made to eliminate the non-functional pads.  Most of 
the time it is allowed (which makes us happy).  Sometimes it is not.

The presence of nonfunctional pads on high layer count PCB's has been argued 
to increase the z-axis dimensional stability of the hole walls (reduction in 
foil cracking).  Leaving the unused pads on the board is simply a non-value 
added band-aid for excessive z-axis expansion of the laminate system.  The 
solution is not to leave these pads on the design but to remove the 
non-functional pads and use a higher Tg laminate which has a lower z-axis 
expansion.

The absence of non-functional pads

1.  decreases the cycle-time in the AOI (automatic optical inspection) 
operation

 This is the case because there is less copper on the etched panel. 
 Scanning time is not affected.  What is affected is the quantity of 'false 
calls' found by the AOI equipment.  'False calls' are locations where the 
AOI machine detects an error but which are usually the result of oxidation 
of the surface copper on the core changing the reflectivity of the copper. 
 A greater degree of these 'false calls' means a greater amount of time 
verifying their validity, and therefore the cycle-time for the AOI 
operation.


2.  increases overall hole quality for the vias.

Higher layer count products tend to utilyze smaller via drill sizes.  The 
resulting high apsect ratio, combined with a large quantity of copper which 
must be drilled through causes the via holes to be somewhat funnel-shaped. 
 The reason for this is as follows.  Optimally, the chip (debris) is carried 
out of the hole along the flute of the bit and does not impact the hole 
wall.  Practically, this does not happen since the chip, before it has a 
chance to escape the hole, leaves the flute and impacts the hole wall.  The 
impacting of copper chips on the hole wall causes the hole to be somewhat 
funnel-shaped.  The process is streamlined to minimize the  funnel-shape by 
useing a bit which has a negative taper (the bit is larger at the end that 
hits the hole first) and the infeed of the drill is alterred to try to pull 
the chip out of the hole along the flute.  However, a good CAM-level method 
for reducing the funnel-shape is to rmove the source of the abrasive action, 
namely the non-functional pads.


Steve Silbert
Product Engineering Manager
Automata, Inc.
[log in to unmask]