Mark, On 1mm pitch BGA, I prefer using 19.3 mil pad & 10 mil drill dia. Trace & clearence of 5 mil in outer layer. For inner layer it's 4 mil trace & spacing. This is my personal thinking & not official. Trilok -----Original Message----- From: icu-pcb-forum-bounce@xxxxxxxxxxxxx [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx]On Behalf Of Mark Salberg Sent: Thursday, February 16, 2006 7:33 PM To: icu-pcb-forum@xxxxxxxxxxxxx Subject: [PCB_FORUM] Re: BGA Fanout / Filled vias On my 1mm BGA, I have an 18mil BGA pad and (18mil via pad, encroached to 14mil with a 8mil hole). BGA pad (not mask) to via encroachment = 11.8mil. However, the assembler specified "copper to copper" which would be "airgap" pad to via measurement. Copper to copper / airgap = 9.8mil. The via encroachment to ball copper pad (not larger mask) sounds like what they should spec. Is this a correct statement? Looks like he may be in the "Ball-park" with the filled vias for .8mm and below pitch BGA's. On my .75mm BGA I have: 6.5mil ball pad to encroached via. airgap = 4.5mil. (same for mask to encroached mask on via) = 4.5mil. Our thought was that if there is a soldermask dam, then there should be no paste wicking in the via. But with 10mil min airgap, they must be filled and possibly tented. When you epoxy fill the vias, do you also tent the vias with mask? Gerry Meier wrote: Mark, If you encroach your vias you would measure from pin to encroachment area. This should give you enough Pin to Via/Encroachment (copper to copper) clearance for your Assembler. The formula I have used is for a min 3 mil encroachment is Formula: Pad size diameter - Soldermask opening diameter > or = to 6 mils. But Soldermask opening diameter is not < the drill size (nominal hole size + 3 mils). Sample: 18 mil pad - 11 mil soldermask opening = 7 mil + 9.8 = 16.8 pad to via/encroachment (copper to copper). This may also work for the .75mm BGA however some Assembler's or CM's require BGA's with an .8mm pitch or smaller have their vies plugged under the BGA's. Hope this helps, Gerry Gerry Meier Sr. PCB Designer Freedom CAD Services, Inc. Voice: (603) 864-1300 x1350 AL Voice: (256) 417-6944 Email: gerry.meier@xxxxxxxxxxxxxx Visit us at www.freedomcad.com -----Original Message----- From: icu-pcb-forum-bounce@xxxxxxxxxxxxx [ mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Mark Salberg Sent: Thursday, February 16, 2006 3:25 AM To: Cadence User Group Subject: [PCB_FORUM] BGA Fanout / Filled vias Hello all, What BGA Ball pad to via clearance is needed for BGA fanout? Our Assembly house is telling us that we need 10 mil copper to copper (15mil preferred). On 1mm BGA's using an 18mil via with 8mil drill gets us 9.8mil via to pad. On our .75mm BGA this via gets us 4mil via to pad. Which also breaks the soldermask dam. Is epoxy filled and tented vias our best or only option at this point? Thanks for any input. Mark ________________________________________________________________________ _____ Scanned by IBM Email Security Management Services powered by MessageLabs. For more information please visit http://www.ers.ibm.com ________________________________________________________________________ _____ ----------------------------------------------------------- To subscribe/unsubscribe: Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx with a subject of subscribe or unsubscribe To view the archives of this list please login at //www.freelists.org. Our list name is icu-pcb-forum or go to //www.freelists.org/archives/icu-pcb-forum/ Problems or Questions: Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx Want to post a job listing ? DON'T DO IT HERE! Better yet, join our jobs listing forum. SUBSCRIBE: icu-jobs-forum-subscribe@xxxxxxxxxx POST: icu-jobs-forum@xxxxxxxxxx ----------------------------------------------------------- ----------------------------------------------------------- To subscribe/unsubscribe: Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx with a subject of subscribe or unsubscribe To view the archives of this list please login at //www.freelists.org. Our list name is icu-pcb-forum or go to //www.freelists.org/archives/icu-pcb-forum/ Problems or Questions: Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx Want to post a job listing ? DON'T DO IT HERE! Better yet, join our jobs listing forum. SUBSCRIBE: icu-jobs-forum-subscribe@xxxxxxxxxx POST: icu-jobs-forum@xxxxxxxxxx ----------------------------------------------------------- _____________________________________________________________________________ Scanned by IBM Email Security Management Services powered by MessageLabs. For more information please visit http://www.ers.ibm.com _____________________________________________________________________________ _____________________________________________________________________________ Scanned by IBM Email Security Management Services powered by MessageLabs. For more information please visit http://www.ers.ibm.com _____________________________________________________________________________