Re: [PEDA] BGA Footprint question.
that's pretty small! i would talk to your assembler, i have found that different ones have different opinions Dennis Saputelli Brian Guralnick wrote: Hi everyone, I'm making a 54-BALL VFBGA (8mm x 9mm) package. From a Micron ram chip MT48V8M16LFFF. PDF = http://download.micron.com/pdf/datasheets/dram/MobileY95W_3V_E.pdf In the mechanical package description, it says: 54x /O 0.35 solder ball diameter to post reflow condition. The pre-reflow diameter is /O 0.33. Elsewhere, the spec says that the Solder ball pad: /O .27mm. This is all that we are told with regard to the pad size. Does this mean that the land pattern should be 0.33mm, or 0.35mm? What should the solder mask paste stencil be cut out to? Brian Guralnick [EMAIL PROTECTED] Voice (514) 624-4003 Fax (514) 624-3631 * Tracking #: 709F790AA8A5A04AB22D7874AA0F74C836B673FD * -- ___ www.integratedcontrolsinc.comIntegrated Controls, Inc. tel: 415-647-04802851 21st Street fax: 415-647-3003San Francisco, CA 94110 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] BGA Footprint question.
Brian, as Dennis stated, your assembler should have some good opinions on your question. Other than that, my readings have led me to the opinion that your pad size should match the devices ball pad size, i.e. 0.27 in this case. The theory that sounds the most convincing on matching the ball pad size is that it will give you an even ball distortion between the device package and your board. Mismatched sizes will distort the ball shape and may apply uneven stresses through the ball. Stencil size, that is also dependant on your other pad sizes and thus would have to tie together with your other pads because it would usually be stencilled in one pass. So your pad sizes and the desired volume of paste would dictate the stencil openings for the ball grid and other packages. Sincerely, Brad Velander. Lead PCB Designer Norsat International Inc. Microwave Products Tel (604) 292-9089 (direct line) Fax (604) 292-9010 email: [EMAIL PROTECTED] http://www.norsat.com Norsat's Microwave Products Division has now achieved ISO 9001:2000 certification -Original Message- From: Brian Guralnick [mailto:[EMAIL PROTECTED]] Sent: Monday, September 09, 2002 10:32 AM To: Protel EDA Forum Subject: [PEDA] BGA Footprint question. Hi everyone, I'm making a 54-BALL VFBGA (8mm x 9mm) package. From a Micron ram chip MT48V8M16LFFF. PDF = http://download.micron.com/pdf/datasheets/dram/MobileY95W_3V_E.pdf In the mechanical package description, it says: 54x /O 0.35 solder ball diameter to post reflow condition. The pre-reflow diameter is /O 0.33. Elsewhere, the spec says that the Solder ball pad: /O .27mm. This is all that we are told with regard to the pad size. Does this mean that the land pattern should be 0.33mm, or 0.35mm? What should the solder mask paste stencil be cut out to? Brian Guralnick [EMAIL PROTECTED] Voice (514) 624-4003 Fax (514) 624-3631 * Tracking #: 9B35124B2316D648A86D5987F7329EB693DE707F * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] BGA Footprint question.
Brian, The short version of the answer is neither, the land pattern is the pad, and hence it is 0.27mm. Where in the spec did you get the 0.27mm number? I looked at pages 59 and 60 of the spec and saw that the 90 ball beast actually wants a 0.33mm pad diameter according to Note 2 on page 60. that 0.33mm pad is the land pattern for the 90 ball. As for the 54 ball beast, since the balls are smaller, the 0.27mm sounds right, but I still cant find where you got that number. The 0.33mm number is the actual diameter of the solder ball on the uninstalled part, and the 0.35mm number is the size after it is installed where the ball grows because it gained a little weight as it were, (grew a little) by combining with the solder paste that was on the pad when it is soldered. The mask is critical, and it needs to be as close to the 0.27,, as it can with allowance for misalignment, which obviously can't be much, and I wouls say no more than 1 mil (0.025mm) larger than the pad. It is obvious that the pattern was layed out so that you can access all pads on the top layer without any feedthrus until you get out beyond the ball arrray (or in the middle of it), but your mask also must be big enough to insure coverage of your largest trace. The paste is yet a different issue, and I woild bet that it is certainly no larger than the pad, if not much much smaller. Does the datasheet cover this somewhere else. One problem here is that if your mask is too large here, the board will have extra solder on any trace leading into the pad, which can affect the final ball size by either adding extra solder to the ball from the trace, or reduce the size of the ball by distributing the solder in the ball over a larger exposed area oc plated conductor and pad, all depending on Murphy'd mood (as in Law) on the day that the board is built. They should hactually have an ap note on the paste, besides the datasheet. Have you done a search on their entire site for such an ap note. This would actually be an excellent question for the guys in the IPC TechNet Forum. Hope this has been more help than hinderance, JaMi - Original Message - From: Brian Guralnick [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] Sent: Monday, September 09, 2002 10:32 AM Subject: [PEDA] BGA Footprint question. Hi everyone, I'm making a 54-BALL VFBGA (8mm x 9mm) package. From a Micron ram chip MT48V8M16LFFF. PDF = http://download.micron.com/pdf/datasheets/dram/MobileY95W_3V_E.pdf In the mechanical package description, it says: 54x /O 0.35 solder ball diameter to post reflow condition. The pre-reflow diameter is /O 0.33. Elsewhere, the spec says that the Solder ball pad: /O .27mm. This is all that we are told with regard to the pad size. Does this mean that the land pattern should be 0.33mm, or 0.35mm? What should the solder mask paste stencil be cut out to? Brian Guralnick [EMAIL PROTECTED] Voice (514) 624-4003 Fax (514) 624-3631 * Tracking #: 1A18E8CB74276144BC393CBDA67EC870CF7780C1 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] BGA Footprint question.
paste? i did some 1mm balls they just did a precision application of flux on the lands, no paste the balls just reflowed Dennis Saputelli Brad Velander wrote: Brian, as Dennis stated, your assembler should have some good opinions on your question. Other than that, my readings have led me to the opinion that your pad size should match the devices ball pad size, i.e. 0.27 in this case. The theory that sounds the most convincing on matching the ball pad size is that it will give you an even ball distortion between the device package and your board. Mismatched sizes will distort the ball shape and may apply uneven stresses through the ball. Stencil size, that is also dependant on your other pad sizes and thus would have to tie together with your other pads because it would usually be stencilled in one pass. So your pad sizes and the desired volume of paste would dictate the stencil openings for the ball grid and other packages. Sincerely, Brad Velander. Lead PCB Designer Norsat International Inc. Microwave Products Tel (604) 292-9089 (direct line) Fax (604) 292-9010 email: [EMAIL PROTECTED] http://www.norsat.com Norsat's Microwave Products Division has now achieved ISO 9001:2000 certification -Original Message- From: Brian Guralnick [mailto:[EMAIL PROTECTED]] Sent: Monday, September 09, 2002 10:32 AM To: Protel EDA Forum Subject: [PEDA] BGA Footprint question. Hi everyone, I'm making a 54-BALL VFBGA (8mm x 9mm) package. From a Micron ram chip MT48V8M16LFFF. PDF = http://download.micron.com/pdf/datasheets/dram/MobileY95W_3V_E.pdf In the mechanical package description, it says: 54x /O 0.35 solder ball diameter to post reflow condition. The pre-reflow diameter is /O 0.33. Elsewhere, the spec says that the Solder ball pad: /O .27mm. This is all that we are told with regard to the pad size. Does this mean that the land pattern should be 0.33mm, or 0.35mm? What should the solder mask paste stencil be cut out to? Brian Guralnick [EMAIL PROTECTED] Voice (514) 624-4003 Fax (514) 624-3631 * Tracking #: 9B35124B2316D648A86D5987F7329EB693DE707F * -- ___ www.integratedcontrolsinc.comIntegrated Controls, Inc. tel: 415-647-04802851 21st Street fax: 415-647-3003San Francisco, CA 94110 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] BGA Footprint question.
No choice. The very low power SDRAMS have very small packages. You know, for PDAs other ridiculously compact devices. Thankfully, there are only 54 contacts, not something like 500-1000... Brian Guralnick [EMAIL PROTECTED] Voice (514) 624-4003 Fax (514) 624-3631 - Original Message - From: Dennis Saputelli [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] Sent: Monday, September 09, 2002 1:54 PM Subject: Re: [PEDA] BGA Footprint question. that's pretty small! i would talk to your assembler, i have found that different ones have different opinions Dennis Saputelli Brian Guralnick wrote: Hi everyone, I'm making a 54-BALL VFBGA (8mm x 9mm) package. From a Micron ram chip MT48V8M16LFFF. PDF = http://download.micron.com/pdf/datasheets/dram/MobileY95W_3V_E.pdf In the mechanical package description, it says: 54x /O 0.35 solder ball diameter to post reflow condition. The pre-reflow diameter is /O 0.33. Elsewhere, the spec says that the Solder ball pad: /O .27mm. This is all that we are told with regard to the pad size. Does this mean that the land pattern should be 0.33mm, or 0.35mm? What should the solder mask paste stencil be cut out to? Brian Guralnick [EMAIL PROTECTED] Voice (514) 624-4003 Fax (514) 624-3631 * Tracking #: 709F790AA8A5A04AB22D7874AA0F74C836B673FD * -- ___ www.integratedcontrolsinc.comIntegrated Controls, Inc. tel: 415-647-04802851 21st Street fax: 415-647-3003San Francisco, CA 94110 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
