If you're doing flip chip designs there's more to the story. Mask defined pads are almost mandatory because the solder mask registration tolerance can be a show stopper with fine lines and spaces, say typically 50/50 micrometres. More importantly the mask defined pad guarantees a specific pad surface area for more consistent paste reflow cross-section because there are no traces of none or varying widths open to taking some of the reflowed solder away from the flip chip ball. These traces can absorb a significant percentage of the total solder volume and open the possibility of starving the flip chip ball, leading to possible long term reliability problems. And the characteristics of the reflowed solder paste will change depending on which direction the mask registration is off, whether it increases or decreases the amount of open solder stealing copper. All tricky when your pads are 150um diameter on 300um pitch.
A significant factor is the presence of the solder mask edge under the reflowed ball. As Paul says, there are stresses involved at the solder mask edge that can cause ball cracks with thermal cycling over a period of time. Many years ago we did a study about this exact problem and found that if the solder mask thickness was kept below 20um (0.8mil) then there were no significant stresses on the ball even after HAST reliability testing. We also found that the sharpness of the corner of the solder mask on the upper surface contributed to joint failure, but it was very hard to consistently provide a 'soft' corner for the mask without other problems rearing their ugly heads.
However, I think it would be a good idea to do your own testing. We did some cool things in those days and there may have been other factors involved, like die size, number of balls, thermal environment, substrate thickness etc. However there is no doubt our mask defined pad tests were valid.
Cheers.........
AndyK
0424 432 235
-----Original Message-----
From: DesignerCouncil [mailto:[log in to unmask]] On Behalf Of Pete
Sent: Saturday, 22 March 2014 02:50
To: [log in to unmask]
Subject: Re: [DC] Microvias in pad
You should avoid mask defined BGA pads, if possible. Avoiding any mask overlap on the pads is a good idea. The problem isn't solder slumping over pad edges (it doesn't do that anyway), it's the mask creating a solder to pad joint shape that concentrates stress. If your intermettalic is always good, and the PCB isn't stressed much, you should be OK, but there's no margin for error.
Use the manufacturer's pad size, the via in the pad will be plugged, you don't really need special considerations in mask or paste for this application. The mask size will be some compromise considering your PCB fabricators copper and mask location and aperture tolerance and minimum mask web capability that keep mask off the pads. The assembler should control the paste aperture based on their process.
Pete
---------------------------------------------------------------------------------
DesignerCouncil Mail List provided as a free service by IPC using LISTSERV 16.0.
To unsubscribe, send a message to [log in to unmask] with following text in the BODY (NOT the subject field): SIGNOFF DesignerCouncil.
To temporarily stop/(restart) delivery of DesignerCouncil send: SET DesignerCouncil NOMAIL/(MAIL) For additional information, or contact Keach Sasamori at [log in to unmask] or 847-615-7100 ext.2815
---------------------------------------------------------------------------------
______________________________________________________________________
This email has been scanned by the Symantec Email Security.cloud service.
For more information please contact helpdesk at x2960 or [log in to unmask]
______________________________________________________________________
---------------------------------------------------------------------------------
DesignerCouncil Mail List provided as a free service by IPC using LISTSERV 16.0.
To unsubscribe, send a message to [log in to unmask] with following text in
the BODY (NOT the subject field): SIGNOFF DesignerCouncil.
To temporarily stop/(restart) delivery of DesignerCouncil send: SET DesignerCouncil NOMAIL/(MAIL)
For additional information, or contact Keach Sasamori at [log in to unmask] or 847-615-7100 ext.2815
---------------------------------------------------------------------------------
|
