Jack, we pwb manufacturers keep adding names that mean the same thing to
confuse the general public. Once they have learned all the names, we then
use the substitute acronym to confuse them even more. Anyway I'll try and
de-mystify the questions that you pose :
Prepreg = B-stage = bond sheets
These three identical meaning words deal with a raw material used in pwb
manufacturing. Specifically prepreg, as it commonly referred to, is a woven
glass fabric (E-glass) that has been dipped in a liquid epoxy (also known as
A-stage). After this impregnation (hence the name prepreg) the liquid coated
cloth is dried so that the epoxy solidifies. The material is then cut to a
specific size and used as one of the layers used to bond (glue) together the
inner layers in a multilayer sandwich. It is important to note that the
material at this stage (B-stage) is NOT FULLY cured but merely ready to be
chemically converted to it's polymerized state (or C-stage) at the
lamination process.
Core
A core or thin core, is simply one or more layers of the B-stage prepreg
noted above, that has been laminated between two layers of copper foil. By
selecting the number of prepreg layers and the glass fabric thickness, you
can manufacture cores of varying thickness. At this point the core should be
fully cured and is also known as C-stage.
Cure buzzwords :
A-stage - liquid epoxy resin ready for coating onto glass fabric
B-stage - dried, uncured, epoxy resin coated on glass fabric
C-stage - Fully cured B-stage prepreg coated with sheets of copper foil
Thickness specifications:
The best response for this question is to work with your pwb manufacturer.
The pcb manufacturing process is fraught with details and there are so many
details implicated in your question that it may be unwise to provide
guidelines. In general, the specification for thickness variations can be
found in MIL-S-13949. This is a generic military specification for all types
of B-stage and C-stage materials. A general rule of thumb is that you can
generally get what you want... for a price. The tighter the tolerance, the
more expensive the materials. Generally designers specify only overall
thickness and, when necessary, specific dielectric thicknesses and
tolerances are generally only specified when electrical performance demands
such.
Warpage:
Unbalanced stackups are constructions that are not evenly balanced about the
theoretical midplane of the board. In your example, one of the layers of
copper would be much higher copper density than the other layers. This
results in a disproportional volume or resin (I often say that resin is the
root of all evil) in that specific inner layer, in relation to the other
layers. As a result, the resin shrinkage that naturally occurs, causes an
imbalance in shrinkage in the X-Y plane. If this difference is substantial,
the result is warped substrates. In order to remedy this, simply add copper
thieving or 'pseudo-pads' on the associated layer in order to reduce the
difference in copper area to less than 10% difference. After completing this
the amount of resin at each layer would be balanced and the resulting
shrinkage equally dispersed in the substrate.
I hope that these words reduce your confusion. Please RSVP if this is still
not clear.
Dave Rooke
Circo Craft - Pointe Claire
_________________________________________
>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
>
>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.
>
>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"...
>
>Thanks in advance, Jack
>
>***************************************************************************
>* 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. *
>***************************************************************************
>
>
>
***************************************************************************
* 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. *
***************************************************************************
|
