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.
> ----------
> From: George Franck[SMTP:[log in to unmask]]
> Reply To: TechNet E-Mail Forum.;George Franck
> Sent: Tuesday, January 09, 2001 2:00 PM
> To: [log in to unmask]
> Subject: Re: [TN] Unused Inner Layer Pads: Remove or Not?
>
> Good afternoon,
>
> I have to provide another perspective on this.
>
> I assume that your pad stack is designed with the smallest pads possible,
> which allows for
> layer-to-layer registration errors, material shrinkage, drilling accuracy,
> annular rings,
> etchback, and all the other gremlins in the PWB Fabrication process that
> keep the drilled
> holes from being drilled exactly in the center of the padstack. Lets look
> at what removing
> the Non-functional pads can get you.
>
> Lets use an example, Your hole size in set up for a .0135 drill. You
> want 1 mil annular
> rings (internal), and you are allowing the PWB house .010 for their
> tolerance build ups. So
> the minimum pad size is going to be .0255. Lets steal the half mil from
> the Fab house.....
> and use .025 pads.
>
> Now, You, or the supplier, is going to put the .0135 hole and .025 pad in
> their test coupon.
> And they will use this coupon and make a cross section to verify that the
> drilled hole is
> where is should be, ie at least .001 from the edge of the pad (annular
> ring).
>
> The Cross section demonstrates that the edge of the hole stays inside a
> .023 diameter area, at
> least in that cross section.
>
> Lets go back to the design process. You are routing the board, and your
> design rules say you
> must maintain a .003 minimum space. If you run a trace too close to a
> pad, your CAD tool will
> register a "line to pad" spacing error. So all traces are kept .003 from
> the edge of the pad,
> and .004 from the edge of the hole.
>
> Now, lets remove the Non-functional pads, and rout traces. Some routers
> will now allow you to
> rout traces in the area once occupied by the non-functional pad. (This is
> the reason you
> wanted to remove the non-functional pads, i.e., to squeeze traces into
> places they dont
> fit..) If a trace is now routed .020 from the center of the hole, a
> spacing error is not
> generated.
>
> Remember the Allowances we gave the supplier. The hole can be anywhere
> within a .023 diameter
> area. The hole could be drilled thru this trace, and be within its
> mechanical tolerances.
> These dead shorts will be identified at electrical test. The reliability
> problems are the
> holes that are very close to the traces. They are not shorting out today,
> but given some
> humidity and some time.... ZAP!
>
> In my ever so humble opinion, (IMESHO) the non-functional pads can be
> reduced to a minimum
> size, (0 annular ring requirement) during the layout and rout design
> process. In this case,
> the pads are effectively a "keep out" area, representing the area where
> the drilled/plated
> hole may occur. The pads will help your CAD tool maintain your minimum
> spacing requirements.
> You should never rout a board without non-functional pads present. I
> suppose you could set up
> keep outs in your pad stack to do the same thing as non-functional pads,
> in which case, my
> concerns go away.
>
> After routing is complete, and all Design Rule Checks are completed, there
> may be some
> advantages to removing these pads.
>
> In my experiences as a PWB fabricator, we usually left the Non-functional
> pads in. There are
> agruments either way about non-functional pads in the fabrication process,
> and I am 100%
> behind any position my current boss takes. Before routing your traces,
> however, keep the pads
> IN.
>
>
> George Franck
>
>
> The reason fractions prevail and the Dewey Decimal system never caught on
> in America?
> Well...... that is because Truman beat Dewey... remember?
>
>
> Franklin D Asbell wrote:
>
> > Remove them all...provided of course your customer has no problem with
> > that.
> >
> > What you might learn later in fabrication is that the handful you
> > thought were not an issue has just bit your butt. Besides, if they're
> > unused, why use them ~grin~
> >
> > Franklin
> >
> >
> --------------------------------------------------------------------------
> -------
> > 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
> >
> --------------------------------------------------------------------------
> -------
>
> --------------------------------------------------------------------------
> -------
> 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
> --------------------------------------------------------------------------
> -------
>
---------------------------------------------------------------------------------
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
---------------------------------------------------------------------------------
|
