John:

You should review the responses again.  I only skimmed them, but they
appeared to address pads on inner layers only.  Removing pads on
external layers will leave you open to potential reliability problems
for several reasons:

1.  An artwork dot or pad approximately the drilled hole diameter is
required on outer layers where there is no pad.  This allows plating in
the hole.  The size of this feature affects the thru hole plating.  If
the pad is at the drilled hole size, the plating will reach the surface
but any misregistration will result in a partial annular ring on the
board surface.  As the feature's diameter becomes smaller, the plating
in the hole barrel recedes from the outer surface of the board to a
point where there is little or no plating in the hole.

2.  The adhesion of a plated barrel to laminate is not always optimum. 
See specifications on resin recession for what is allowable.  If
separation occurs at the outer layer, you have a pocket that can collect
contaminates or worst case propagate the separation through the board. 
Boards that have been subjected to a desmear process (almost all
multilayers) will exhibit greater adhesion of the hole barrel to the
laminate compared to the same board without desmear (primarily double
sided).

3.  Consider where the board will be probed after assembly.  A via
without an outer layer pad and plating that does not reach the surface
might not reliably make contact with a test probe.

In conclusion, the benefits of retaining or removing internal pads are
well represented by the following responses, but the removal of external
pads IMO is not recommended.  Rather follow the guidelines in IPC-D-275
for pad sizing allowing for breakout per IPC-6012.

Don Vischulis
[log in to unmask]

[log in to unmask] wrote:
> 
>      Tom/All,
> 
>      Unless I miss understood your email, it should not matter if you leave
>      or omit pads with regards to drill stack height, unless you are 2nd
>      drilling (which is scarce these days).  Your primary drill is done
>      into a blanket of copper.  Your copper weight is nominal across the
>      panel, so lands, conductors and pads are irrelevant to drill stack
>      height.
> 
>      CONCLUSION:
> 
>      What I am gathering from the responses is that the forum (industry),"
>      including myself, have always used pads with annular rings (the "we
>      always have" syndrome applies here).  No one's at fault, we all have
>      established our own Fabrication and Assembly standards that are
>      specific to our Industry or product.  Eventually the standards  become
>      obsolete and fall to the way side.  And after all the testing and
>      statistical data, we ask ourselves, "Why did we ever do that."  The
>      answer is never as obvious as we want to be.
> 
>      I initially theorized that the external pads (A/R) were necessary to
>      support the material expansion in the Z-axis.  Doing so would minimize
>      the amount of possible circumferential voids.  Some of this was proved
>      in past thermal shock testing (200-400hrs @85°C).  As later explained,
>      this has some volatility.
> 
>      Lyle Dove has another avenue of thought that makes sense.  The
>      internal pads (A/R) minimized the amount of hole wall peel.  You can
>      use the analogy, "nothing solders better than solder."  Or,
>      electroless deposition would adhere better to the exposed copper
>      layers than to the catalyst/laminate.
> 
>      Werners response is helpful, but my decision to omit lands from the
>      design are driven by real-estate constraints and not reliability.  I'm
>      assuming the gain he speaks of is non-functional gain and omitting
>      lands causes potential problems.  Could you further explain Werner?
> 
>      And last, I spoke with Marshall Andrews at ITRI in Austin, Texas and
>      we reviewed the recent (Round Robin) Study entitled "PWB Hole to Land
>      Mis-Registration," (#97061201-G).
> 
>      A synopsis of the results:
> 
>      1. Leaving or omitting the land, internal and external, has no affect
>         on the end product reliability (there's a catch).
>      2. CATCH - The external pad does assist in minimizing the amount
>         Z-axis expansion due to the CTE mismatch of copper and laminate.
>         This failure was typically found at about 600 - 1000 hrs Thermal
>         Cycling.  This is outside the scope of many products.
>      3. Internal lands did not provide more support to minimizing peeling
>         as with no lands.
>      4. Mis-registered drilled vias/pths (breakout) did not affect the
>         reliability any worse than dead centered or annular ring.
>      5. Drilled holes in the egress (conductor/pad junction) had no bearing
>         in the reliability.
> 
>      So there you have it.  Thank you all for your support.
> 
>      If information on items 1-5 is discrepant with what was discussed and
>      read from the above study, I apologize to Marshall Andrews.  Please
>      forward any direct.
> 
>      John Gulley - Process Quality Engineer
>      Inet Inc.
>      1255 W. 15th Ste 600
>      Plano, TX 75075
>      972-578-3928
> 
> _____________________________ Reply Separator _________________________________
> Subject: RE: FAB: Padless vs. Padded
> Author:  [log in to unmask] at Internet
> Date:    7/16/97 9:56 PM
> 
>           I agree wholeheartedly with Werner's statement and
>           conclusion that the possible gain in reliability is not
>           worth the loss in manufacturability.  In some cases, if the
>           non-functional pads are required to be left on, drill stack
>           height is reduced and this impacts board cost.  The round
>           robin study is also quite outdated (I believe the late
>           '80's), and was done at a time when small hole drilling was
>           new to everyone.  There have been several process
>           enhancements since then.  Hmmmmm....maybe it's time to do a
>           new study?!?
>           Tom Coyle
>           Field Services Engineer
>           HADCO Corporation

***************************************************************************
* TechNet mail list is provided as a service by IPC using SmartList v3.05 *
***************************************************************************
* To subscribe/unsubscribe send a message <to: [log in to unmask]>   *
* with <subject: subscribe/unsubscribe> and no text in the body.          *
***************************************************************************
* If you are having a problem with the IPC TechNet forum please contact   *
* Dmitriy Sklyar at 847-509-9700 ext. 311 or email at [log in to unmask]      *
***************************************************************************