Bob Vanech wrote:-
>       The original question was in respect to larger internal pads in
>   their designs and why, since we have never seen or done that ourselves.
>   I was just interested in the rational that went into making that design
>   requirement for possible implementation into our product line if like
>   requirements occur.
>
>        After all is said and done, the message is: Whatever set of design
>   parameters are generated, communicate with your fabricator NOW to reduce
>   problems later.

Hi Bob,

I commend your last para and hope all on the forum are of like mind.

In the original question, if you want to know why larger pads on
internal layers are a good idea, read on and please forgive me if this
is too simplistic.

Basically the main problem with inner layers is the registration of the
drilling to the inner layer pattern. The extra tolerances which have to
be considered are:-
Photo-Tool stability 0.1 mil per inch
Laminate movement    0.25 mil per inch
Layer to Layer alignment 2 mil
Core to Core alignment   2 mil
Tooling hole accuracy for drilling 2 mil
Drilling machine tolerance 1 mil
                (The above will vary with fabricator and board spec)

The registration of the outer layers is affected by the first and the
last but not those in between and so the tolerance has to be greater
for internal layers. It follows that the pad sizes must be greater for
inner layers than for external layers.

The main reason is not breakout. The most important reason is to make
sure the clearance between the plated holes and any adjacent copper is
not reduced below the minimum specified which I would say should be not
less than 7 mils. If the inner layers are designed with 2 mil land and 7
mil space, the fabricator will need to increase the space to around
(say)14 mil to achieve a minimum of 7 mils on the finished pwb's.
A prototype or pre-production batch could be manufactured with less
clearance on a smaller panel and achieve acceptable yield, but it would
be more expensive to produce in production quantities.

The alternative is to make the minimum land 9 mils and the space 7 mils
to ensure that there is no possibility of breakout. This is much better
than making the minimum land 2 mils and the spacing 14 mils for obvious
reasons. It is just a question of how to achieve the end result without
causing undue restrictions on the track density. Making the lands bigger
is a neat solution although the reason may not be obvious.

Please don't forget the hole is a copper conductor and the clearances
must make allowance for the registration variations. Putting pads of
suitable size on all holes will make the layout much better and the
unconnected pads can always be deleted later by the fabricator. And if
you can't fit everything in to the space available, consider adding an
extra couple of layers.

I hope this is clear but if there is any question about this please let
me know.
--
Paul Gould
Teknacron Circuits Ltd
[log in to unmask]
Isle of Wight,UK


--
Paul Gould
[log in to unmask]
Isle of Wight,UK