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

This would actually be an excellent question for the guys in the IPC TechNet

Hope this has been more help than hinderance,


----- 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 =
> 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
> Voice (514) 624-4003
> Fax (514) 624-3631

* Tracking #: 1A18E8CB74276144BC393CBDA67EC870CF7780C1

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* Contact the list manager:
* Forum Guidelines Rules:
* Browse or Search previous postings:
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to