Mike,
        My intent in doing this is to allow me to maintain .006 trace
widths, .006 spacing ( .005/.005 finished) in my design without reducing my
pad size to a degree that it makes it difficult to maintain annular ring.

        The problem connector has .040 pads on a .050 pitch. Here're the
pad/hole requirements:
        A)  .013-.019 finished holes.
        B)  2 x  .002 annular ring internal
        C)  2 x .002 etchback
        D)  .012 mfg. allowance

        So that  tells me I need a minimum pad of .039. Without reducing my
requirements or increasing the manufacturing difficulty it seems to me I
gain a lot by removing unused pads. Routing a 6 mil trace down a 10 mil slot
gives me 2 mils per side of clearance. By removing the unused pads my trace
is now (worst case) 4 mils from the edge of the barrel, and nominally my 6
mil trace is 25 mils from the center of an 18-20 mil barrel.
        That sounds like a big improvement to me, or am I missing something?
-Mike Hiteshew

> ----------
> From:         Mcmaster, Michael[SMTP:[log in to unmask]]
> Reply To:     TechNet E-Mail Forum.;Mcmaster, Michael
> Sent:         Wednesday, January 10, 2001 2:05 PM
> To:   [log in to unmask]
> Subject:      Re: [TN] Unused Inner Layer Pads: Remove or Not?
>
> I'm probably saying the same thing as George.  The critical part of your
> question is that your asking if you can remove the pads to increase wiring
> density during layout.  The answer is absolutely not.  Remember what the
> pad
> is for, to make an interconnect to the drilled hole.  The reason it's
> larger
> than the hole is to make sure the hole is still in the pad when all the
> manufacturing tolerances are taken into account.  The non-functional pad
> means there's no interconnect on that hole on that layer, but the drilled
> hole will still be there.  The non-functional pads are friendly reminders
> to
> keep traces out of that area.
>
> If you need more room, you need to ask two question of your board
> fabricator
> and one of yourself.  For the fabricator, the first question is "how much
> larger than the drilled hole must a pad be and still capture the hole"?
> The
> second is "what's the minimum pad to trace space they can etch?"  For you,
> "from a reliability viewpoint, what's the minimum conductor-to-conductor
> spacing I want in the finished board?"  Take the larger of the answers to
> the last two questions and add it half the answer to the first.  If you a
> run a trace closer to a hole than that, your fabricator will be throwing
> them away for shorts at electrical test or you'll have boards which don't
> meet your reliability expectations.
>
> For example, your fabricator says I need a pad 0.010" larger than the
> drilled hole and I can etch a 0.004" space.  You follow IPC and want a
> minimum 0.0035" spacing.  You should put in the desired pad size (while
> your
> at it, if you're cutting it this close, you might as well find out the
> exact
> drill bit diameter they will use).  Then rout traces with a minimum 0.004"
> spacing.
>

---------------------------------------------------------------------------------
Technet Mail List provided as a free service by IPC using LISTSERV 1.8d
To unsubscribe, send a message to [log in to unmask] with following text in
the BODY (NOT the subject field): SIGNOFF Technet
To temporarily halt delivery of Technet send the following message: SET Technet NOMAIL
Search previous postings at: www.ipc.org > On-Line Resources & Databases > E-mail Archives
Please visit IPC web site (http://www.ipc.org/html/forum.htm) for additional
information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700 ext.5315
---------------------------------------------------------------------------------