Tom, One assumes you are talking about 'microvia-in-pad' VIP and not drilled through-hole via-in-pad. The drilled TH's definitely need to be plugged with a plated surface cap, The microvias can be filled or not depending on price and fabricator capability. From a design alternative, the via can be in the center of the pad or off-center at the edge. It can be just off the pad and covered with soldermask (called an 'Inset microvia') or it could be a dogbone connection (we assume there is no room for this or it would have been done already). Solectron did some assembly studies about the voiding with 'microvia-in-pad' and had a few conclusions. Their report had a number of good cross-sections about the issue. The key is to get all the parties talking early to decide what the trade-offs are. There need not be a problem if the issue is flushed out early enough. SOLECTRON VIA IN PAD STUDY * Via partially in pad show little voiding compared to the offset via configuration. Center via configuration had the most voiding. Inset and dogbone via, little if any voiding. * Large amount of voiding were observed on ENIG surface finish boards. Very few on immersion silver. * Smaller the pad size, more the voiding. Generally, voiding defects(%) for 0.5mm CSPs were higher than 0.8mm CSPs. Voiding on 1.0mm BGAs were minimal. * Next build will focus on the contribution of paste, reflow profile, Air/N2 atmosphere to voiding. This process was standard SMT. Need to investigate other micro-via construction techniques like filled via, etc. * Lead-free soldering may make the problem worse. I have a couple of reports that have a lot of pictures and illustrations on the issue and alternative solutions if you want. Send me an email if you would like them, I will give you an FTP Box to download them from. They are to big for emailing. Happy Holden Westwood Associates Tom Parkinson <[log in to unmask]> Sent by: DesignerCouncil <[log in to unmask]> 06/25/2004 11:14 AM Please respond to "(Designers Council Forum)"; Please respond to Tom Parkinson To: [log in to unmask] cc: Subject: [DC] VIA in Pad We're a CM. One of our customers is asking us to build a board assembly that will be using BGAs with VIAs in pads. They are in the design stages at this point, and we have some concerns with having a Via in the middle of a BGA pad. Anyone have suggestions and/or experience with this?? Thanks Tom Parkinson - Quality System Manager - CIT WinTronics, Inc. Ph: 724-981-5770 Ext. 235 Fax: 724-981-1772 --------------------------------------------------------------------------------- DesignerCouncil Mail List provided as a free service by IPC using LISTSERV 1.8d To unsubscribe, send a message to [log in to unmask] with following text in the BODY (NOT the subject field): SIGNOFF DesignerCouncil. To set a vacation stop for delivery of DesignerCouncil send: SET DesignerCouncil NOMAIL Search previous postings at: www.ipc.org > On-Line Resources & Databases > E-mail Archives Please visit IPC web site http://www.ipc.org/contentpage.asp?Pageid=4.3.16 for additional information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700 ext.5315 ---------------------------------------------------------------------------------