Stephen, It depends right? For .80 mm pitch BGA components you could use the following. BGA land = .40 mm (15.748032 mils) Blind Via in pad = .15 mm hole (5.905512 mils) Solder mask clearance around BGA land of .13 mm (5.11811 mils) This would result in a .14 mm (5.511811 mils) soldermask dam between the BGA lands. Tenting vias is risky as you said, so you could call out for a type VII via, (filled and capped) this would allow a flying probe tester to test the via also. Again, it depends upon your budget, design, your board vendor .... etc. Donald Kyle C.I.D.+ At 06:36 AM 11/16/2007, you wrote: >*Currently our PCB designs utilize "encroached" solder mask via pads on >pin escapes for all of our products. >This was an adequate treatment for products with 1.27mm but as BGA lead >pitch starts shrinking, the issue of adequate solder dams between ball >pads and their pin escape vias becomes more problematic. >Our standard pin escape via pad is typically .024" with .012" Finished >Hole Size (FHS). Our requirement is solder mask encroached 1:1 with FHS. >*First dilemma is that fabricators require .006" solder mask clearance >over primary drill size. >*This yields .001" solder mask encroachment on a .024" via pad with a >.012" FHS under ideal conditions with no mask misregistration. >*Problem becomes more pronounced with .8mm BGA pin escape vias. Our >typical pad geometry for .8mm BGAs is .016". The pin escape via pad >diameter for these devices is typically .018". That will yield only >.005" clearance between the via pad and adjacent BGA pad. If fabricator >requests .006" over primary drill, that leaves 0 solder mask on pin >escape via pad with perfect solder mask registration. Problem is further >exacerbated when fabricators increase solder mask apertures to >accommodate misregistration and prevent solder mask from getting onto >SMT pads. This results in as little as .003" solder dams. >*Predict that there will be an abundance of issues whenever parts need >to be reworked. > Our preferred PCB surface finish is ENIG with SMOBC construction. >*Typical practice in industry is to "tent" over vias with LPI. However, >this practice is problematic and can lead to long-term PCB reliability >issues. >*Tenting vias with LPI solder mask will cause ENIG plating chemistry to >become entrapped in vias. >I would like to know how others are handling vias under BGA's with a >pitch of .8mm or less. > >If we plug our vias we will have the following issues: > >* > Via fill process will increase cost of PCB and will potentially >increase lead time as well. >* > *Need to have vias covered with solder mask on BGA placement >side to prevent potential for solder wicking onto via land. This becomes >very critical during rework operations. > >* > *Need to have vias exposed on non-placement side for test >access. > >* > *Vias filled with non-conductive media will cause probe contact >issues during flying probe and In-circuit test. > >* >Any help would be appreciated > >Stephen J. Mariani >Mercury Computer Systems, Inc. >199 Riverneck Road >Chelmsford, MA 01824 >Phone: 978-967-1855 >Cell Phone: 978-761-4101 >Fax: 978-244-0520 >Email: [log in to unmask] > > > >--------------------------------------------------------------------------------- >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 temporarily stop/(restart) delivery of DesignerCouncil send: SET >DesignerCouncil NOMAIL/(MAIL) >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 >847-615-7100 ext.2815 >--------------------------------------------------------------------------------- --------------------------------------------------------------------------------- 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 temporarily stop/(restart) delivery of DesignerCouncil send: SET DesignerCouncil NOMAIL/(MAIL) 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 847-615-7100 ext.2815 ---------------------------------------------------------------------------------