Michael,
        while I can generally agree with your advice you leave one aspect
wide open. If you do not specify your layer thickness, you could get a board
that works fine from manufacturer A, switch to manufacturer B and have a
board that doesn't work fine. The problem, one manufacturer used a stack up
with inter-layer thickness X, manufacturer B used inter-layer thickness Y
and the board now has different impedance, inductance characteristics. In a
lot of designs this would not cause a problem but then there could be that
one slightly longer clock trace or other timing or very level transition
sensitive signal which may not meet specs and cause a board failure. You ran
thousands of boards from one manufacturer and they worked fine, purchasing
changed manufacturers, ordered 10,000 and now none of them work reliably. Or
the techs nightmare, 50% of them fail but very unreliably.
        Specifying just the minimum prepreg thickness does not give you any
control over the repeatability of that design and therefore does not meet
the IPC condition that any manufacturer should be able to build a "working"
version of your PCB. If you do not specify your total laminated prepreg
thickness, you are rolling the dice. I know of some manufacturers who will
by default use a 30 - 40 mil core, others will use a 20 mil core, if you do
not think this is significant to your design, that 'may' just be because you
don't know your design well enough. It is not always a matter of specifying
only for controlled impedances, it is a matter of specifying such that you
can get a reliable 'known' product from multiple manufacturers as the IPC
spec suggests.

Brad Velander,
Lead PCB Designer,
Norsat International Inc.,
#300 - 4401 Still Creek Dr.,
Burnaby, B.C., V5C 6G9.
Tel. (604) 292-9089 direct
Fax (604) 292-9010
website www.norsat.com


> -----Original Message-----
> From: Michael Reagan [mailto:[EMAIL PROTECTED]]
> Sent: Monday, July 09, 2001 8:28 AM
> To: Protel EDA Forum
> Subject: Re: [PEDA] Layer Stackup Info.
> 
> 
> Jeff,
> 
> Word of advice...and this is a rule and a fab note we use for 
> all designs.
> We specify  a MIN  core and prepreg  thickness for all 
> layers, in one fab
> note. We spec .0035 inch min.   This gives your fabricator 
> the latitude to
> adjust for copper distribution, laminates he has in stock, epoxies,
> pressing, over all thickness variations, etc.  The only 
> conditions in which
> we specify a thickness and we only spec it for these layers, 
> are controlled
> impedance, and where the min dielectric breakdown voltage is 
> required for
> Bell-Core, FCC, and space applications.   My advice is to 
> leave the majority
> of your stack up determined by your board house, unless you 
> have specific
> reason to do otherwise.
> The IPC spec in 6012 for level 3 is to specify a design so 
> that any board
> house can build your design with the same result.   Remember you are
> designing/ writing  a specification,  give the fabricator 
> some latitude
> 
> 
> Mike Reagan
> EDSI
> Frederick  MD

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*                      - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to