TECHNET Archives

January 2001

TechNet@IPC.ORG

Options: Use Monospaced Font
Show Text Part by Default
Show All Mail Headers

Message: [<< First] [< Prev] [Next >] [Last >>]
Topic: [<< First] [< Prev] [Next >] [Last >>]
Author: [<< First] [< Prev] [Next >] [Last >>]

Print Reply
Subject:
From:
"Mcmaster, Michael" <[log in to unmask]>
Reply To:
TechNet E-Mail Forum.
Date:
Wed, 10 Jan 2001 17:44:02 -0800
Content-Type:
text/plain
Parts/Attachments:
text/plain (101 lines)
Mike

In this particular case it does buy you a little bit because of your 0.002"
annular ring requirement.  That's "free" space that you can get rather
easily.  I still have some concern about going to all the trouble of having
the board built to IPC Class 3, presumably for reliability concerns, then
designing to allow the trace to be only 0.004" from the barrel.

> ----------
> From:         Hiteshew, Michael[SMTP:[log in to unmask]]
> Sent:         Wednesday, January 10, 2001 1:31 PM
> To:   'TechNet E-Mail Forum.'; 'Mcmaster, Michael'
> Subject:      RE: [TN] Unused Inner Layer Pads: Remove or Not?
>
> 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
---------------------------------------------------------------------------------

ATOM RSS1 RSS2