From: Zabinski, Patrick J. ([email protected])
Date: Fri Feb 02 2001 - 04:51:34 PST
Jan,
I have not seen or had any experience with the particular E-PBGA
technology you're looking at, but here are a few answers
based on what I have seen (sorry, I don't have answers to
all your questions).
> -b- what is the material used for PBGA and E-PBGAs? An idea
> of the permitivity?
PBGAs utilize a wide array of dielectrics. Based on the fact
that you can see the buried layers, my guess is that the substrate
is based on a build-up (vs laminate) process (at least for
the outer/upper layers). This being the case, the most commonly
used dielectrics usually range from 3.8 to 4.2. If the package
is based on a laminate technology, the most common dielectrics
are generally a bit higher (due to glass content?), say 4.0 to 4.6.
> Common track widths?
Most PBGAs today allow for 75 micron (3 mil) widths for common traces with
necking down to 50 or 60 microns (2-2.5 mil) in a few areas. However,
just like PCBs, the larger you can keep the geometries, the easier
it is for them to make, the less expensive the resulting package will be.
> -d- need the layer buildup be symmetric, as in PCBs?
In a laminate technology, the answer is most-often Yes. You'll
need to keep the buildup symmetric for the interconnect/plane
layers to keep the substrate flat during processing. They'll
then add the heat spreader to the back.
In a build-up process, the answer is most-often No. They generally
start with a sheet of copper (heat spreader) and build up the
layers sequentially from there. Most build-up processes do
not require an even number of layers or the layers to be symmetric.
> -e- where can I find design rules for these kind of packages?
> Any on-line??
Most vendors do not publish their capabilities on-line. You'll
likely need to pick a vendor and speak directly with them
about their rules.
> -f- similar as -e-, who makes layout tools for these kind of
> packaging?
There use to be a tool specific to designing BGAs where all you
did was enter in a few parameters (# I/O, die size, etc.), and it
would do all the routing for you. If your die/system requires
optimum electrical performance from a BGA, you'll most likely
be better off using a different tool where you hand-route
the traces.
For hand-routing, any PCB design tool will work. All BGA vendors
I've dealt with in the past few years have accepted Gerber data
(one exception; a vendor required DXF, which I generated by
translating Gerber into DXF).
If you do your own design, keep in mind that the manufacturer will
be of great help in providing valuable input on how to design the
package for producibility (i.e., cost). However, I have yet to
find a BGA vendor that truly understands SI and how the BGA
design can dramatically effect how the overall system operates.
Hope this helps,
Pat
**** To unsubscribe from si-list or si-list-digest: send e-mail to
[email protected]. In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu
****
This archive was generated by hypermail 2b29 : Tue May 08 2001 - 14:30:48 PDT