[log in to unmask]"> I cannot resist this one....From a board manufacturer's point of view, inner layer and outer layer pad concerns are completely different.
The process of imaging and etching an inner layer involves: the photoresist being applied to an undrilled core material, then the exposing and developing of it. This positive image is then put through an etcher and this is the inner layer image, without holes. Then the cores are laminated and the board is drilled. If a board has 4,000 holes, and 50 traces on an inner layer signal layer, I would rather deal with 50 traces only, than 50 traces and 4,000+ pads. When the board is completed, a hole with no pads on the innerlayers would be no different (or have no less integrity) than a hole on a non-multilayer board. If the processes are under control, there should be no problem with the holes. The material used in making a double sided board is manufactured in the same was as a multilayer board is built, with prepreg and foil (basically).
As far as the outer layers go, small (< .150, say) non plated holes with pads that are intentional, must be processed differently (an extra step) than non plated holes without pads. AND, if you have a large non plated hole with small pad (<.015 per side over hole size), the pads can randomly pop off, for various reasons.
I think the general opinion of most fab houses is this: Data comes in from so many different systems, it is hard to know if there were restrictions on the data output, or if many of the situations are intentional. If the fab house has a strong front end system all issues are addressed, and the boards are built to the customer's requirements. I can say that from a yeild point of view, though, most all builders of PCB's would rather delete unused pads on inner layers, and have no pads on outer layer Npth holes.
Regards,
K BergmanGenny Gibbard wrote:
Fascinating stuff. We had a board vendor at one point that wanted us to put
pads on all the layers of a PTH. I thought the reason given was to help the
hole plating process. Our standard block for multilayer boards
automatically puts pads on all layers and if not a ground via, it also
clears the ground plane away around it on all layers. I've never heard of
any of the problems mentioned over the last few days.
It's kind of funny, the amount of things I hear about on this forum that
question things or dispute things that we've never really paid much
attention to in our own layouts makes me fascinated that this co. has gotten
as much product out the door working as it has over the last dozen years. I
guess Murphy's law isn't always on duty.-----Original Message-----
From: Hinners Hans M Civ WRALC/LUGE [ mailto:[log in to unmask] ]
Sent: January 17, 2002 4:03 PM
To: [log in to unmask]
Subject: Re: [TN] Remove unused "dead" pads on internal layersHi All,
Now that I think of it we always stuck our nonfunctional pads in places we
didn't have to drill. But I'm on the list to learn - thanks to Warren,
Werner.Roger, this sounds very weird - granted I've only been in the industry since
'98. There are very good reasons to use nonfunctional pads. Now I know not
to use them in PTHs (& Route areas I imagine). I wonder if people are
making this more difficult than it has to be - we've always used decent
sized dots so they wouldn't pop off of the core from rough handling or
processing. We kept them far enough away from traces to avoid etch problems
- we're not talking about something that has to have a critical feature
size. They may have been struggling with metallic contamination but
non-functional pads should be a fixable problem - no?If they were truly having problems with non-functional pads then they must
have had the same trouble with the functional pads? Houston . . . . we've
had a problem.Hans
Integrity First - Service Before Self - Excellence in All We Do
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
Hans M. Hinners
Electronics Engineer
Warner Robins - Air Logistics Center (WR-ALC/LUGE)
226 Cochran Street
Robins AFB GA 31098-1622Com: (478) 926 - 5224
Fax: (478) 926 - 4911
DSN Prefix: 468-----Original Message-----
From: Roger M. Stoops [mailto:[log in to unmask] ]
Sent: Wednesday, January 16, 2002 2:10 PM
To: [log in to unmask]
Subject: Re: [TN] Remove unused "dead" pads on internal layersI have been following this thread with interest. When I asked a pcb vendor
about having non-functional pads in the inner layers, they said it was not
a good idea, that the unattached pads/lands would move around, or "float,"
and cause potential mfg problems, such as shorts to other copper.
Question: Is there any truth to this statement, or is this just an old
husband's tale?
TIA,
Roger M. Stoops, C.I.D., PCB Designer
[log in to unmask]Trimble
Engineering and Construction Division
5475 Kellenburger Rd.
Dayton, OH 45424-1099 USA
Ph: +01 937.233.8921 or +01 937.233.4574 ext 288
Fax: +01 937.233.7511"<Peter
George To: [log in to unmask]
Duncan>" cc:
Sent by: Subject: Re: [TN] Remove unused
"dead" pads on internal layers
TechNet
<TechNet@IPC.
ORG>01/15/02
09:09 PM
Please
respond to
"TechNet
Forum.";
Please
respond to
peter.duncanHi,
Actually these "unused" pads are replicates of the hole "rules" created for
the surface layers. Most routing packages, or routers, seem to do this by
default for each layer to save manual replication where traces, etc are to
be connected. (At least PADS, Alegro and Mentor do). On the grounds that
it's always easier to destroy than to build, it's easier to delete pad data
than to create it, so it's put in by default as there's a good chance it
will be needed.I still say you should consider hole barrel strength/support issues before
just deleting them - e.g. they can constrain the "resin recession" and hole
wall pull-away that have been recent threads on this forum. Think of the
"unused" pads as 'wall ties' holding the copper at frequent intervals to
the hole wall. Copper bulging or pull-away in the event of recession or
whatever is reduced.Peter Duncan
Hinners Hans M Civ
WRALC/LUGE To: [log in to unmask]
<Hans.Hinners@ROBI cc: (bcc: DUNCAN
Peter/Asst Prin Engr/ST
NS.AF.MIL> Aero/ST Group)
Sent by: TechNet Subject: Re: [TN] Remove
unused "dead" pads on
<[log in to unmask]> internal layers01/15/02 09:40 PM
Please respond to
"TechNet E-Mail
Forum."; Please
respond to Hinners
Hans M Civ
WRALC/LUGEHi Patrick,
As others have said, I don't think the class of board matters for "unused"
pads. It all depends on what your procurement documentation states, are
you
building to drawing or is there a clause that says process improvements
that
do not affect functionality are permissible."Are they really unused pads?"
They may be electrically nonfunctioning but they are there for a reason -
better lamination quality (avoiding low pressure areas or excessive prepreg
flow), better hole wall quality, better plating quality (esp. for any
isolated traces), reduced loading of your etch solution or better thermal
loading during assembly.Hans
Integrity First - Service Before Self - Excellence in All We Do
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
Hans M. Hinners
Electronics Engineer
Warner Robins - Air Logistics Center (WR-ALC/LUGE)
226 Cochran Street
Robins AFB GA 31098-1622Com: (478) 926 - 5224
Fax: (478) 926 - 4911
DSN Prefix: 468-----Original Message-----
From: Patrick Lam [mailto:[log in to unmask] ]
Sent: Friday, January 11, 2002 5:12 PM
To: [log in to unmask]
Subject: [TN] Remove unused "dead" pads on internal layersHi TechNetters,
For class 3 boards, is it acceptable to have unused pads removed on
interanal
layers.Thanks,
Pat----------------------------------------------------------------------------
-----
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 e-mail to [log in to unmask]: SET
Technet NOMAIL
To receive ONE mailing per day of all the posts: send e-mail to
[log in to unmask]: SET Technet Digest
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 e-mail to [log in to unmask]: SET
Technet NOMAIL
To receive ONE mailing per day of all the posts: send e-mail to
[log in to unmask]: SET Technet Digest
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 e-mail to [log in to unmask]: SET Technet NOMAIL
To receive ONE mailing per day of all the posts: send e-mail to [log in to unmask]: SET Technet Digest
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
---------------------------------------------------------------------------------