PCB Assembly Services - Screaming Circuits: 0.4mm pitch BGA pads


0.4mm pitch BGA pads

At 0.5mm pitch and larger, we generally recommend non-solder mask defined (NSMD) pads for BGAs. The NSMD pad will allow for better adhesion with the solder being able to grip the sides of the copper in addition to the top surface. Even down to 0.5mm pitch BGAs, most part manufacturers still say to go with NSMD pads. Granted, you need to make sure your fab house can do a good job of mask registration. It's no good to have pads that are half SMD and half NSMD. We've seen that.

Once you go down to 0.4mm pitch BGAs, though, things get different. We're starting to see more and more of these. Some CSP (chip scale package) or WSP (wafer scale package) BGA and LGA parts are starting to show up in 0.4mm pitch, as well as some bigger parts like the Ti OMAP processor.

At that size, you start to see more risk of solder bridging with NSMD pads, as in the left side of the illustration below.
0.4mm pitch SMD BGA pads 
This is a somewhat exaggerated view, but it shows the potential problem here. With such small geometries, you probably aren't going to be able to route escape traces on the top layer either. You'll have to put blind vias in the pads and escape through the inner layers. By the way - NO OPEN VIAS IN PADS. The pad needs to be solid metal with such a part. No exceptions. Don't try using solder mask to cap the vias at this pitch either. Plate over it. It has to be all metal.

You can finds some more detail here in a design guide written by Ti for their OMAP processor. Pages 8 through 12 talk about pads, mask and vias. Obviously, you should consult similar materials written specifically for the part you are using, but Ti did a great job of covering all the issues here so I use it as a good general piece.

Duane Benson
Are you there Moles? It's Edgar.


TrackBack URL for this entry:

Listed below are links to weblogs that reference 0.4mm pitch BGA pads:


Dave - I checked the link and it worked on my system. Here's the actual URL. You can try it directly: http://www.ti.com/lit/an/spraav1b/spraav1b.pdf

Hi Charles; The IPC recommends that the exposed solderable area of the land on the PCB match to size of the pad on the BGA that the ball is attached to. By their standards, the registration can be off far enough that up to 1/4 of the soldermask is off the pad. In my opinion, that's not good enough for the small pitches.

I would follow your same 3 mil rule of thumb, making sure that the exposed copper area matches the copper land area on the BGA package. If that ends up removing too much clearance between pads, you could reduce that while maintaining the same exposed copper area and ask for a higher registration tolerance form your PCB fab shop.

How do I need to account for soldermask registration? When I do NSMD, I add 6 mils (3 on each edge) to the pad size to be sure no mask gets deposited on the pad.

In the case of SMD, should the copper pad extend 3 mils on each side beyond the mask opening? Or can I just have the mask opening the same size as the copper pad?

The link has been fixed - as of 4/20/2010, anyway.

the link to the design help is no longer valid

"You can finds some more detail here in a design guide written by Ti for their OMAP processor"

Post a comment

If you have a TypeKey or TypePad account, please Sign In.

« Beavers and Ducks at ESC last week | Main | Short-Run Parts »