The relevant variables for determining the pad size for a drilled hole are:

Pad Size = Drill Size + Registration Budget (from your PCB Fabricator)  +
twice the minimum annular ring requirement

For example if you have 13.5 mil drill, your fabricator requires a 8 mil
registration budget (4 mils per side) and you have a 1 mil annular ring
requirement you should put a 23.5 mil pad on the IL for the drilled hole.

As for trace proximity to the hole, it is slightly dependent on whether you
decide to leave non-functional pads (NFPs) on the IL.  The most important
factor is the distance between the drilled hole wall and the trace.  The
desired value should be specified somewhere.  This is one of the areas where
the IPC specs are confusing.  IPC relegates this requirement to the annular
ring specification.  This seems to be only half the requirement especially
since annular ring breakout is allowed.  You also need to know the minimum
spacing required between the pad and trace, especially for routing traces.

Again, an example.  You have a 1 mil annular ring requirement and a design
with three mil pad-to-trace spacing.  At maximum misregistration, this will
result in a 4 mil space between drilled hole wall and the trace. Is this
adequate?  I don't know and IPC 6012 does not appear to address it.

Even worse is if you allow hole breakout on the pad.  For IPC 6012 class 2,
you can have 90 degree breakout.  In theory this breakout means you can use
a smaller pad for a particular hole size.  Because the amount of breakout is
a function of the pad and hole diameter, I'll use a larger hole for this
example.  If you are using a 30 mil drill, you are allowing approximately
1.5 mils of breakout ( had to break out my Perry's handbook and calculator
to figure that one out).  From above, you know your fabricator requires 4
mils of annular registration.  The 1.5 mils of breakout can be deducted from
this, therefore you make your pad 35 mils (2.5 mils per side larger than the
drill).  Now you set the pad-trace spacing at 3 mils on the auto router, sit
back and watch.  The problem is you end up with traces that are only 5.5
mils from the edge of the perfectly registered hole and only 1.5 mils away
from the hole at the maximum annular misregistration of 4 mils!  I don't
know anyone who will claim that this is adequate separation between hole and
trace.

"So what does this have to do with removing non-functional pads?" you ask.
I'm starting to wonder about that myself.  The relevance is that the
distance between hole and trace at maximum misregistration is the critical
parameter for how close you can run traces to drilled holes regardless of
whether you use pads or not.  Therefore there appears to be no advantage to
removing the NFPs, then doing the routing.  In fact there is a big
disadvantage if you forget to set the hole to trace spacing at the necessary
distance.  I have even on occasion seen a trace run right through the
drilled hole location.  What I usually recommend is that the NFPs be left in
the design until all the routing is completed.  The pad serves as a "keep
out" for traces.  Remove the pad after the design is complete.

The only possible advantage I can see to removing the pads then routing is
that if your combined minimum annular ring and pad-trace designed spacing
exceeds the minimum hole-to-trace spacing required on the finished board.
One last example.  You have a 2 mil annular ring requirement and the board
is designed at 5 mils pad-trace spacing.  Your minimum requirement for hole
to trace is 4 mils.  If you leave NFPs in when routing you would have a
minimum pad-trace of 7 mils on the finished board.  Removing the NFPs will
buy you an extra 3 mils of routing space.

> ----------
> From:         Olson, Jack[SMTP:[log in to unmask]]
> Reply To:     TechNet E-Mail Forum.;Olson, Jack
> Sent:         Wednesday, April 26, 2000 10:18 AM
> To:   [log in to unmask]
> Subject:      [TN] PCB FAB: bending the rules?
>
> Sorry for the cross-post, but I couldn't decide if this was more of a
> fabrication issue or a design issue.
>
> We typically remove unused pads from inner layers. (please don't change
> the
> subject to warn me against removing inner-layer pads, that's not the issue
> I
> need help with right now)
> I am being asked to use the extra routing space that has been freed up by
> the pads being removed. I have heard of this before but never tried it,
> and
> frankly I'm a little worried about it.
>
> Somewhere I heard that the gap between traces to the drilled hole should
> be
> something like 11-15mils, but that hardly makes sense from what we are
> already doing. A 13mil via hole in a 25mil pad is probably drilled with an
> 18mil drill bit, right? If we were already using a 4mil clearance to the
> 25mil pads, then removing the pad still only leaves 7mils to the edge of
> the
> drilled hole right? (sorry for all the numbers in one sentence)
>
> So how much extra routing space is there? I say virtually none. I can't
> remember where I heard that drill to route should be 11-15mils, has that
> become tighter these days?
>
> Anyway, that brings up another question. Maybe we can use smaller pads on
> inner layers? That's yet another thing I've never tried....  Is there a
> rule
> of thumb for that or am I just asking for trouble?
>
> Any responses will be greatly appreciated
>
> Jack
>
> ##############################################################
> TechNet Mail List provided as a free service by IPC using LISTSERV 1.8c
> ##############################################################
> To subscribe/unsubscribe, send a message to [log in to unmask] with
> following text in
> the body:
> To subscribe:   SUBSCRIBE TECHNET <your full name>
> To unsubscribe:   SIGNOFF TECHNET
> ##############################################################
> Please visit IPC web site (http://www.ipc.org/html/forum.htm) for
> additional
> information.
> If you need assistance - contact Keach Sasamori at [log in to unmask] or
> 847-509-9700 ext.5315
> ##############################################################
>

##############################################################
TechNet Mail List provided as a free service by IPC using LISTSERV 1.8c
##############################################################
To subscribe/unsubscribe, send a message to [log in to unmask] with following text in
the body:
To subscribe:   SUBSCRIBE TECHNET <your full name>
To unsubscribe:   SIGNOFF TECHNET
##############################################################
Please visit IPC web site (http://www.ipc.org/html/forum.htm) for additional
information.
If you need assistance - contact Keach Sasamori at [log in to unmask] or
847-509-9700 ext.5315
##############################################################