hi brad and darcy i have done some .8mm pitch BGA, but the company it was for went under before it got built :)
but at your dimensions your only real choice is via in pad there just isn't room for a fanout drilled hole i have heard of 8 mil starting drill but that still doesn't get you there these BGAs definitely drive up layer counts the laser vias have various technologies that go only to the next and also all the way through it's hard to imagine the supporting circuitry being happy with a 2 layer board anyway, i suspect you will be looking at 6+ layers i hope the power is clustered in the middle ! make friends with your fab house as you will probably be married to them after this 3 mil traces are getting very common now but brad is correct that the reliability is suspect your assembler will need to do 100% XRAY (or other more advanced) inspection what is the function of this part ? i don't suppose they make a bigger one ? Dennis Saputelli _______________________________________________________________________ CONTACT INFORMATION: _______________________________________________________________________ Integrated Controls, Inc. Tel: 415-647-0480 EXT 107 2851 21st Street Fax: 415-647-3003 San Francisco, CA 94110 www.integratedcontrolsinc.com _______________________________________________________________________ NOTE! TO PASS OUR SPAM FILTER PUT THE FOLLOWING IN SUBJECT LINE: I.C.I. Brad Velander wrote: > Hi Darcy, > Here is my take on your questions. I haven't actually used this > technology yet but I believe a few others here have. You may very well hear > from them as well. > > 1) Sure 3mil traces and spaces are do-able by some specialty shops but I > would sooner put fanout vias between the pads and route out on another layer > using more reasonable 4/4mil or larger routing. 3/3mil will just get you > stuck in a high tech board fab issue with other associated failures because > of the tiny Cu topology. > > 2) Yes! It actually is used when referring to both (rightly or wrongly), > so further detail is needed to be sure you differentiate between the two. It > can also describe small diameter vias in the pad with no fill. There they > rely on the minimum diameter and reflowed solder viscosity to stop solder > wicking away from the pad. > > 3) Yes there definitely are limits so a conversation with the target > fabricator would be in order. Some are limited to very thin single layers but > some are doing 2 layers, maybe 3 thin layers. It is not the same as regular > vias though so make sure you get the full technical scoop from the target > fabricator. > > 4) The talk with the fabricator is also in order for this question. Don't > forget though that your first row out doesn't need any clearances and that a > number of your internal row pads could use regular via technology. Therefore > greatly reducing the number of routes requiring clearances on the first > internal layer. Don't forget to look eagerly for any unused pins as well, > utilizing those spots for additional routing room or fewer vias required. > > > Sincerely, > Brad Velander > Senior PCB Designer > Northern Airborne Technology > #14 - 1925 Kirschner Road, > Kelowna, BC, V1Y 4N7. > tel (250) 763-2232 ext. 225 > fax (250) 762-3374 > > > > -----Original Message----- > From: Darcy Davis [mailto:[EMAIL PROTECTED] > Sent: Thursday, October 19, 2006 4:12 PM > To: PEDA ([email protected]) > Subject: [PEDA] Suggestions on BGA layout > > > Hey folks, > > We're about to delve into our first design with a real BGA. I've certainly > been able to find a few helpful documents online, but I thought I'd run a > couple questions past this knowledge base. The part is an 84 pin VFBGA with > a ball dia. of 0.3mm (nominal) and a pitch of 0.5mm (~20mil). The array is > 10x10 with a 4x4 area in the center with no balls (this leaves three "rows" > of pads around the outside of the component). We're trying to balance the > cost of new PCB technologies with the risk of poor solder joints, so I'm > looking for some recommendations. > > Just so you know where we're coming from, we're currently doing 2-4layer > boards with 10/26mil vias and 4/4mil trace/space. We do most designs with > 0.062" FR4, but have done 20, 30 and 40mil thicknesses as well. No laser > drilled or blind/buried vias. > > 1) The manufacturer recommends a 260u pad (~10mil), leaving a gap of 240u > (~9mil) between pads. For fanout, we're considering doing 3 mil traces with > a 3 mil spacing. Is this reasonable? Will this technology likely be less > expensive then microvias or other fanout alternatives? > > 2) Does "via-in-pad" refer to a microvia within a pad? or does it > specifically refer to a via that has been plugged to prevent solder wicking? > I assume they can plug using a conductive material as opposed to epoxy? Is > it reasonable to assume that this isn't applicable to our part since > microvias don't need plugging and conventionally drilled vias would be too > big? > > 3) Could we put a microvia all the way through a 2-layer 40mil PCB? 60 mil? > or is their a limit to the thickness one can laser drill? (Therefore > limiting its use to 4-layer boards only). > > 4) The mfgr recomends "via-in-pad" as a preference to routing out on the top > layer. What size of annular ring is necessary on the inner layer for a > microvia? If the inner layer pad has to be 10 mil, we're still limited to > 3/3mil trace/space to get the middle row of signals out. Sounds like an > expensive endeavor when you account for microvias and 3/3mil traces. > > Hmm. That should at least get me going. Has anybody got a fanout of a > similar BGA that they would be willing to share? I'm just really shakey on > the "right" way to fanout a BGA using micro/blind/buried vias. Thanks in > advance. > > Darcy Davis > > > > ____________________________________________________________ > You are subscribed to the PEDA discussion forum > > To Post messages: > mailto:[email protected] > > Unsubscribe and Other Options: > http://techservinc.com/mailman/listinfo/peda_techservinc.com > > Browse or Search Old Archives (2001-2004): > http://www.mail-archive.com/[email protected] > > Browse or Search Current Archives (2004-Current): > http://www.mail-archive.com/[email protected] > > ____________________________________________________________ You are subscribed to the PEDA discussion forum To Post messages: mailto:[email protected] Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[email protected] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/[email protected]
