Vincenzo, In addition to what you listed in your mail, you will also need to consider the clearance hole (antipad) around the pad, which may be at least 8 to 10 mils bigger than the pad. Adjacet signal vias would completely perforate the plane. I agree with Lee's comment he made earlier on this thread: 0.8-mm BGA is tough on conventional PCBs with through holes. You may need a build-up process or sequential lamination to get your routing properly. Regards, Istvan Novak SUN Microsystems ----- Original Message ----- From: "Vincenzo Kreft-Kerekes" <vincenzo@xxxxxxxxxxxxxx> To: "Tayyab Jamil" <tayyab@xxxxxxxxxxxxxx> Cc: <si-list@xxxxxxxxxxxxx> Sent: Monday, December 29, 2003 9:25 AM Subject: [SI-LIST] Re: 0.8mm BGA routing > Tayyab, > > You're right, I apologize. It looks like you need a 16 mil via pad to route > 5/5 between two vias which in turn makes for a tiny drill hole (8 mil > probably) and all its associated plating problems. Could someone comment > please? Thanks. > > Regards, > Vincenzo > > -----Original Message----- > From: Tayyab Jamil [mailto:tayyab@xxxxxxxxxxxxxx] > Sent: Monday, December 29, 2003 12:54 AM > To: Vincenzo Kreft-Kerekes > Cc: si-list@xxxxxxxxxxxxx > Subject: RE: [SI-LIST] Re: 0.8mm BGA routing > > > 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 > > > ------------------------------------------------------------------ > 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 > > ------------------------------------------------------------------ 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