-- [ From: Doug Jeffery * EMC.Ver #2.5.1 ] --
------
Jack Olson Wrote:
> Subject: FAB DWGS - Specifying Material/Stackup
> I am a circuit board designer, and would like to ask a few questions
to any
> board fabricators out there...
>
> Question 1 (difficulty:easy)
> Can someone briefly summarize the difference between B-Stage, Laminate
,
> Pre-preg, Core and Bonding Sheets (and any other commonly used words
related to
> board material)? I keep getting confused
B-stage = pre-preg = bonding sheets, are the fiberglass sheets coated
with the appropriate resin system (fr4, polymide, etc.) dried but not
cured, and are used to bond innerlayer cores and final layer foils in a
lamination process.
Laminate = Cstage = Core, are the cured raw materials used to create
internal layers and are usually copper clad for creation of circuit
patterns.
> Question 2 (difficulty:challenging?)
> As a circuit board designer using only FR4 and no impedance control,
how
> accurately should I specify material thicknesses? I have seen fab dwgs
that
> have the exact material type (some kind of code) and thickness for
every layer,
> and other dwgs specify only the finished board thickness. Our drawings
say
> "minimum dielectric thickness .0035" but I'm not sure why. Do we have
to
> declare a minimum for some reason? Should I pay more attention to
stackups than
> I have in the past? Its seems to me that the vendors know what types
of
> material are available and can judge how to build a board based on
their
> experience, I haven't had any problems just noting the finished
thickness (that
> I know of, anyway), and I usually trust that they know what they are
doing
> (don't laugh). OK, maybe I am leaving too much to chance, but can
someone
> enlighten me as to why a designer would call out EXACTLY what to use?
Seems
> pretty limiting and possibly needlessly expensive, and a rather time-
consuming
> study that I would rather not undertake unless there is a reason for
it.
You probably have the .0035" min. dialectric space left over from the
old Mil-P-55110 requirement of .0035" min. For years that was a
constant in our industry...we sure shot that all to pieces...
With no electrical requirements you can simple show the layer sequence
on your drawing using names that match your design files and most
fabriators should give you a "balanced" construction from the center of
the board out...They will do this because it is the most economical and
it controls warpage the best...If you need to controll some z-axis
aspect of the design than add that requirement to the drawing...
>
> Question 3 (difficulty:not sure)
> I have read several messages discussing board warpage, and that a
primary
> reason for it is unbalanced construction. OK, I understand that, but
what if I
> have a design with three routing layers and one ground plane? Should I
try to
> offset warpage by calling out a thicker material on one side or the
other? Just
> curious if there are things I can do to "counter-balance"...
Most fabricators can "balance the copper by use of flow patterns and
dams in the border of the panel to off set the 3 signal layers and 1
ground layer...provided you are using normal copper weights .5 oz. and 1
oz. If you speicify 2 oz grounds and 1 oz signals you could have a
real problem.. but matched 1 oz layers or .5 oz layers are probably
workable at the fabrication level...DO NOT offset the layers let the
fabricator use his knwoledge of his abilities to figure out how to
control the flatness of the panel.
Douglas Jeffery
Electrotek, Inc.
[log in to unmask]
414-762-1390
***************************************************************************
* TechNet mail list is provided as a service by IPC using SmartList v3.05 *
***************************************************************************
* To unsubscribe from this list at any time, send a message to: *
* [log in to unmask] with <subject: unsubscribe> and no text. *
***************************************************************************
|
