Technetters,
At this point I want to present my position, because I have one. But first - the trigger to my question came from a failure analysis I made to a batch of 12 boards. We manufactured nearly 200 units of this relatively new product without significant problems. Yes, we have had some, but we assumed they were related to the complexity of the board (18 layers, 15 BGAs, 5000 components total, 4 mils traces and spaces, 2.7 mm thick, controlled impedances on all the layers, and a bunch of other goodies). But this specific batch failed completely. Since the assembly was done in two runs, while the PCB batches in each assembly run were mixed (2 to 3 PCB batches per assembly run) and the problem was only on the bare boards from the specific batch we concluded that the problem is in this batch.
The problem in the assemblies was that on every board there were few (1 to 5) disconnected traces. In one of the cases we drilled down to the identification of the via that while pressing on the failure disappeared. We made a cross section through this via and found a very nice plating, with uniform coating (nice task, considering the 1:9 aspect ratio of this thick board) - and a clear horizontal crack right in the middle of the Z-axis. Also, it was clear from the analysis that all the non-functional pads were removed.
The Gerber data contains the pads in all the layers. We allow removal of non-functional only with our consent because of two reasons:
1. Via strength and withstanding of thermal cycles.
2. Sometimes the pad is being used as a trib for signal integrity, if so needed by the high speed signal analysis simulations (3.125 GHz, after all).
I think that in this case the first reason proved itself to be valid. Since the PCB manufacturer disagreed with me (hello there, I know you read it!) I decided to ask for the honored forum opinion.
Regards
Ofer Cohen
Manager
Quality Assurance, Reliability and Production Technologies
Seabridge Ltd. - A Siemens Company
-----Original Message-----
From: TechNet [mailto:[log in to unmask]]On Behalf Of Mcmaster, Michael
Sent: Tuesday, July 27, 2004 19:26
To: [log in to unmask]
Subject: Re: [TN] Removal of non functional pads
I went back and checked my personal Technet archive. We last discussed this
issue in March 2003. This is my posting from then. (Feel free to check the
on-line archives to see the other posting on this issue - the old subject
was "non functional pad removal")
Begin 2003 post:
So far this argument has been pretty one-sided for leaving non-functional
pads in the design. And I agree with all the arguments presented in favor
of doing so. But there are potential negative impacts to leaving
non-functional pads. Leaving the pads in increases drill wear and heat
generation. As a result drilled hole quality degrades much more rapidly and
defects like pad tearout, hole wall notching, drill bit plugging, etc. occur
much faster. If these aren't being caught, they can be more of a problem
than the reliability gains achieved by leaving pads in. To address this you
need to reduce maximum drill hit counts which ends up increasing the cost of
building the board.
It's important to remember that drilling a circuit board is a very difficult
operation. You are trying to make a very small hole in a (relatively) thick
composite made of dissimilar materials: copper and a glass-reinforced
polymer. And you can't leave any of the latter over the former. The
resulting drill process is a compromise.
A good board fabricator will have done their homework and understand the
interactions involved here. The optimum configuration for NFPs may be a
compromise somewhere between "all" and "none" depending on board thickness,
hole size, material, copper weight, etc.
:End 2003 post
The only thing I'd like to add is my recommendation that you leave the pads
in your design and allow it up to your fabricator whether to leave them in
or remove them. But you do this ONLY AFTER you grill them about their rules
and why they do what they do. The fabricator should be able to support
their position with reliability data.
-----Original Message-----
From: TechNet [mailto:[log in to unmask]] On Behalf Of Frank Kimmey
Sent: Tuesday, July 27, 2004 6:35 AM
To: [log in to unmask]
Subject: Re: [TN] Removal of non functional pads
Ofer,
As you have already seen from Brain, Jeff and others, there are varying
thoughts on this subject.
That said, here are mine.
Unused pads on inner layer can play an important part in the construction
and reliability of your PCBs.
I recommend removal of unused pads on low layer count, low Z axis CTE
materials to improve manufacturability at fab.
There will be longer drill life, less inner layer misregistration
possibilities, etc.
I adamantly refuse to allow removal of unused pads on high layer counts
and/or high Z axis CTE or mismatched CTE materials.
The reasons for this is pretty simple, first if the laminate material
stretches the copper barrel enough then the PTH barrel can actually end up
longer than the PCB is thick (very strange looking phenomena), also
stretching of the plated barrel can cause reliability issues due to cracking
and subsequent opens (read this as field failures).
Leaving at least a minimal annular ring on inner layer pads will aid in
supporting the PTH and reduce the likelihood of damage cause by PCB Z axis
expansion.
I think you will find most fabricators would prefer to see unused pads
removed as that will commonly improve manufacturability, where most
reliability types would prefer to see all pads remaining to improve barrel
anchoring/strength and integrity.
Talk to your fabricator and your quality guys to help reach the best
decision for your specific construction.
Remember communicate your issues and most of them will have an acceptable
solution.
Hope it helps,
FNK
Frank N Kimmey CID+
Principle PCB Designer
Powerwave Technologies
EDH 916-941-3159
FAX 916-941-3195
CEL 916-804-2491
-----Original Message-----
From: Ofer Cohen [mailto:[log in to unmask]]
Sent: Tuesday, July 27, 2004 3:48 AM
To: [log in to unmask]
Subject: [TN] Removal of non functional pads
Technetters,
Are there any guidelines regarding removal of non functional pads in thick
(>2.5 mm) PCBs? Are the guidelines documented somewhere?
Regards
Ofer Cohen
Manager
Quality Assurance, Reliability and Production Technologies
---------------------------------------------------
Technet Mail List provided as a service by IPC using LISTSERV 1.8e
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 or (re-start) delivery of Technet send e-mail to
[log in to unmask]: SET Technet NOMAIL or (MAIL)
To receive ONE mailing per day of all the posts: send e-mail to
[log in to unmask]: SET Technet Digest
Search the archives of previous posts at: http://listserv.ipc.org/archives
Please visit IPC web site http://www.ipc.org/contentpage.asp?Pageid=4.3.16
for additional information, or contact Keach Sasamori at [log in to unmask] or
847-509-9700 ext.5315
-----------------------------------------------------
---------------------------------------------------
Technet Mail List provided as a service by IPC using LISTSERV 1.8e
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 or (re-start) delivery of Technet send e-mail to
[log in to unmask]: SET Technet NOMAIL or (MAIL)
To receive ONE mailing per day of all the posts: send e-mail to
[log in to unmask]: SET Technet Digest
Search the archives of previous posts at: http://listserv.ipc.org/archives
Please visit IPC web site http://www.ipc.org/contentpage.asp?Pageid=4.3.16
for additional information, or contact Keach Sasamori at [log in to unmask] or
847-509-9700 ext.5315
-----------------------------------------------------
---------------------------------------------------
Technet Mail List provided as a service by IPC using LISTSERV 1.8e
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 or (re-start) delivery of Technet send e-mail to [log in to unmask]: SET Technet NOMAIL or (MAIL)
To receive ONE mailing per day of all the posts: send e-mail to [log in to unmask]: SET Technet Digest
Search the archives of previous posts at: http://listserv.ipc.org/archives
Please visit IPC web site http://www.ipc.org/contentpage.asp?Pageid=4.3.16 for additional information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700 ext.5315
-----------------------------------------------------
---------------------------------------------------
Technet Mail List provided as a service by IPC using LISTSERV 1.8e
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 or (re-start) delivery of Technet send e-mail to [log in to unmask]: SET Technet NOMAIL or (MAIL)
To receive ONE mailing per day of all the posts: send e-mail to [log in to unmask]: SET Technet Digest
Search the archives of previous posts at: http://listserv.ipc.org/archives
Please visit IPC web site http://www.ipc.org/contentpage.asp?Pageid=4.3.16 for additional information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700 ext.5315
-----------------------------------------------------
|
