For flip chips, all of the designs I have ever worked with in the past 20 years have been with no soldermask at all inside of the flip chip component area. Typically there is just an open box in the mask, and all of the pads/traces are exposed. We have processed literally millions of flip chips this way, with very, very few failures associated with the flip chips, better than 6 sigma. 
For larger CSP packages where the mask is present under the component, we always use non-soldermask defined pads. For these, misregistration is seldom a problem, provided the fabricator knows what they are doing.
Years ago Werner Englemaier was my manager for a few months on a high-rel flip chip design/development project. He showed me firsthand just how soldermask-defined pads can literally extrude the flip chip solder balls straight up in a vertical manner with only 40 cycles at   -20+100C. We made a benchmark cut, cycled 10 times, performed a microsection across 4 solder balls, cycled another 10 times, made another cut, etc. until we had five successive cuts, using three flip chips on the board. All three components started out with a 2 to 2.5 mil spacing above the soldermask. After 40 cycles they had risen to 4.5 mils, and nearly all of the solder joints had failed. In the first cut, none of the solderballs showed any cracks prior to cycling, but by the time 20 cycles had been completed there were cracks propogating along the pad/ball connection on all of the solder balls in the 3rd cut. 
We only had to make a single cut on the non-soldermask defined samples, and that was after 100 cycles. The microsection on those looked exactly the same after 100 cycles as they did on the initial benchmark cut prior to cycling. 
At that time, I found it hard to believe something as soft as soldermask could possibly put that much pressure on the solderballs, but after I saw those microsections I was forever convinced.


-----Original Message-----
From: DesignerCouncil [mailto:[log in to unmask]] On Behalf Of AndyK
Sent: Friday, March 21, 2014 9:32 PM
To: [log in to unmask]
Subject: Re: [DC] Microvias in pad

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
---------------------------------------------------------------------------------

______________________________________________________________________
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
---------------------------------------------------------------------------------