Some soldermask issues with BGA include ... 1. Mask defined pads are more difficult to cover in one pass during horizontal HASL; a function of surface tension of solder and aperture size. 2. Mask defined pads can lead to long term reliability problems. After reflow the BGA ball conforms to the mask around the pad. A paper by Mike Petrucci (et al) of Compaq showed cracks can form between the BGA ball and PCB pad on mask defined pads. However, their data showed no significant difference in reliability when compared to non-soldermask defined pads (etch defined). Another paper by Dr. Abbas I. Attarwala (et al) of TI showed mask defined pads on the device can lead to failures between the ball and pad. Both situations are caused by the mismatch in Cte between the mask and solder. 3. Etch defined pads with a mask clearance of approximately .003" allow for more solder paste to be printed and possibly a more reliable joint. 4. The clearance between the mask and pad on etch defined pads provides a place for no-clean paste residues to collect after reflow instead of on the PCB surface. 5. Maximize the amount of soldermask between the BGA pad and the connecting via. At BGA rework the mask separating these features can become damaged. If completely removed, reassembly will be difficult since any new paste will run down the via instead of staying on the BGA pad. Regards, D. Mitchell ______________________________ Reply Separator _________________________________ Subject: Re[2]: BGA Author: [log in to unmask] at corp Date: 1/11/96 1:32 PM Doug, Dennis is absolutely right! I've read that anything with I/O >200 is a prime candidate for BGA. Also, the BGA pkg is durable. If accidentally dropped, it can easily be assembled without any potential problem due to the way it's made. (As opposed to a fine pitch/TAB device) I too have seen multiple finish requirements on the same outer surfaces. (As many as 3) Not to mention other temporary protective coatings on top of it. Also the Soldermask clearance on the BGA sites has raised some questions. Some designers are overlapping the pads and others are including clearance and others are 1:1. For the fabricator, it raises a lot of questions. The DFM guidelines for these should be discussed up front to be clearly defined as to the end users requirements. The DFM guidelines for these sometimes goes against what has been used in the past. I know I'm learning, and I understand that the clearance issue is still being evaluated. (From an industry stand point/long term reliability) Groovy ______________________________ Reply Separator _________________________________ Subject: Re: BGA Author: [log in to unmask] at SMTPLINK-HADCO Date: 1/11/96 10:07 AM Doug, First and foremost, get directly involved with your customer at the PCB design stage. The type and quantity of BGA devices will affect layer count, internal and external routing, test-ability, and soldermask apertures. I have seen all types of surface finishes specified; HASL, OSP, hard and soft Ni/Au, and solid solder deposits. I know of one fabricator that supplies BGA product with solder bumps on the all SMD sites but the BGA with the BGA and PTH sites OSP. The assembler does not print any paste, just sticky flux for the SMD's. They're using BGA's with 63/37 balls which supply the solder to the joints. Probably the most significant impact on the PCB fabricator is at electrical test. Depending on your technology level of fixturing software, fixturing, and test equipment, you can easily get into multiple test fixtures that take many hours to solve. Getting involved early in the PCB design can prevent having 4-625 pin CBGA's in a 3"x3" area. Regards, Dennis Mitchell Zycon Corp. [log in to unmask] ______________________________ Reply Separator _________________________________ Subject: BGA Author: [log in to unmask] at corp Date: 1/10/96 5:32 PM -- [ From: Doug Jeffery * EMC.Ver #2.10P ] -- Question? What does BGA technology mean to board fabricators? Do we have to become solder paste experts and reflow solder again.. I thought we got rid of that problem.....:).... No Seriously, what are the responsibilities at fabrication for creating boards to accept BGA's? Thanks? Doug Jeffery Electrotek..