[SI-LIST] Re: 0.8mm BGA routing
- From: Tayyab Jamil <tayyab@xxxxxxxxxxxxxx>
- To: Vincenzo Kreft-Kerekes <vincenzo@xxxxxxxxxxxxxx>
- Date: Mon, 29 Dec 2003 10:54:20 +0500
Vincenzo,
you are perfactly alirght when you mention the space left for pads. but you
did not talk about the tracks escaping between vias.
but when i place vias a matrix form, there is only 31.496 mil distance
between the centers of adjacent via pads. keeping via pad of 20 mil there is
only 11.496 mil space left between the pads of adjacent vias.
Now if i use 5/5 routing this means i need 5+5+5 = 15 mils total space for
routing atleast one track between the pads of adjacent vias, which in our
case is only 11.496. Even 4/4 routing scheme does not allow me to
route/escape one track between the pads of adjacent vias.
I am attaching the rough diagram for reference.
What you say in this regard?
Also please let me know the links/documents reffering to the design of BGAs
with 0.8 mm pitch.
Thanks
Tayyab
-----Original Message-----
From: Vincenzo Kreft-Kerekes [mailto:vincenzo@xxxxxxxxxxxxxx]
Sent: Friday, December 26, 2003 10:19 PM
To: tayyab@xxxxxxxxxxxxxx
Subject: [SI-LIST] Re: 0.8mm BGA routing
Tayyab,
You place escape vias diagonally in the 0.8 mm raster which means you have
0.8 * sqrt(2) = 1.13 mm (44.5 mil) to work with. If you're using a 20 mil
via pad and have an etch capable of resolving 5 mil spaces between copper
structures then you need a 30 mil zone around your via hole center (for pad
and clearance) which leaves 44.5 - 30 = 14.5 mil as pad diameter for the
ball. As was already mentioned, Xilinx has escape diagrams for most if not
all of their packages so you can look at what we're talking about, Altera
also has a good application note on this topic and both have recommended
values for the via and etch parameters in these documents.
Regards,
Vincenzo
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx
[mailto:si-list-bounce@xxxxxxxxxxxxx]On Behalf Of Tayyab Jamil
Sent: Thursday, December 25, 2003 11:35 PM
To: Stephen Chavez
Cc: si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: 0.8mm BGA routing
Hi,
I could not understand your scheme, for me it is not possible what you
suggest as
0.8 mm pitch means there is only about 31 mil distance between via pads of
adjacent pins. 24 mil pad of via leaves only around 7.xx mils space in
between. If we use 5 mil trace this leaves only around 2.xx mils in total on
both sides of the trace, means 1.xx mil clearence on each side of trace.
What i was thinking of is 18mil via pad and 8mil via hole finished, and 4mil
trace and 4mil clearnce. This allows one trace to be escaped between
adjacent pades. Any suggestions about this.
Please let me know if I am wrong.
Regards
Tayyab
-- Binary/unsupported file stripped by Ecartis --
-- Type: application/octet-stream
-- File: Preview PCB1.pdf
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List technical documents are available at:
http://www.si-list.org
List archives are viewable at:
//www.freelists.org/archives/si-list
or at our remote archives:
http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
Other related posts:
