BGA Solder Mask Pull-Back

[Tom Frayda]

Tom-

I was wondering why you've opted to set the diameter of the Solder Mask in your BGA padstacks to be the same as the pad diameter when all of the guidelines I've seen (Lattice, Motorola, Ensil, etc.) recommend a 0.075mm or 0.10mm Solder Mask pull-back (clearance between pad and mask) for NSMD BGA pads.

I can undertand how the larger mask diameter could potentially create inadvertently exposed copper if one were not careful, especially if teardrops are applied. I'm interested in your comments (as well as anyone else's) on the subject.

We're moving toward using BGAs in production applications and I would really like to start off down the optimal path. Thanks.


+Tom

[Tom]

Tom,

This is really a subject that is very similiar to PCB board finishes like NiAu, HASL, OSP, IWT or IAg. What finish is best for you? It's really a matter of what your manufacturer recommends. We use Hallmark Circuits and they put in a IWT line and pulled it out after one month because the tin metal was too harsh on the solermask and they switched to softer metal silver (IAg).

Now in your case, solder mask over the BGA pad recommendations should really come from your assembly shop and not the component manufacturer. Some assembly houses say pull the mask over the pad and some say do not pull the mask over the pad. Get second opinions. Talk to several assembly shops. They give free consulting services. When component manufacturers give you advice, many time the manufacturers disagree with them.

I will do more research in this area and I hope you do too. Let me know what the assembly shops want and I will adjust the solder mask according to their processes.

[Mark Larson]

I thought solder mask pullback was being left up to the fab house? The idea is to have whatever minimum the fab shop is capable of without the mask getting on the pads. I don't see why you would want to generate your Gerbers at 3 or 4 mil pullback if your shop is capable of doing less. If they see you have generated everything at 1:1 but some parts are not, they will probably increase those pads the same as the rest, giving you much more pullback than you really want. They might also put your job on hold until they can get an answer of what you want.

Vendor prints are notorious for having wrong or incomplete information, most are created by someone with little experience or knowledge. Notice many of them are not the document the part is built from.

[Tom Frayda]

Mark-

I typically do not blindly adhere to the recommendations of vendors when it comes to PCB design; more often than not they only get you in trouble.

Normally, soldermask is size on size with the pad in my decal padstacks. However, I raised this question because, when I was researching BGA design, everyone seemed to be saying the same thing about soldermask pull-back for NSMD pads. It began to seem that there may be a valid reason for this (though no one said why) and that it may have an impact on the BGA assembly process. I cite the following resources:

Patrick Johnson, Motorola Inc. - PCB Design Guidelines for BGA Packages

Vern Solberg, Tessera, Inc. - Design for BGA and CSP

Intel BGA Design Guide

Lattice Semiconductor - PCB Layout Recommendations for BGA Packages

Ensil Inc. - BGA the New Kid on the Block

[Mark Larson]

I have read the middle 3 of the 5 resources you cite, and a few more. The most important thing is the ball pad size which should match the metalization pad diameter on the BGA NOT the ball diameter. Very few vendor data include this, most show the ball diameter. This is saddly typical of vendor prints, telling you what you don't need to know and omitting what you need to know. The people that build the boards or assemblies are the people you should talk to, they are the ones that ultimately have to deal with the real world problems, and they can supply the real world answers. Note that the pullback you referenced is 3 to 4 mils, todays standard pullback, although it's fast becoming 2.5 or even 2. A 5 mil pullback would expose the adjacent trace routing, my guess is that it's as simple as that. I doubt any of them would say a 2 mil pullback is not enough.

A great resource for HDI is Dynamic Details Inc., check out their website and attend one of their seminars if you can (free!).

[Tom]

See end post.....

[Tom Frayda]

Thanks for the follow up, Tom!

The recommendations that you received at the conference agree with the IC manufacturer's BGA design recommendations I have seen and referenced... that the solder mask relief should be slightly larger than the pad size (leaving 0.05-0.10mm between the edge of the pad and the edge of the solder mask). I suspected that there had to be a reason behind this.

And, yes, the board manufacurer will have some pull-back based on the tolerances they can hold, but, personally, I feel better if I explicitly design a pull-back into the decal.

Will this information change the way the BGA decals are designed in the pcb standards library?


+Tom

[Tom]

Right now the BGA Solder Mask, in all the BGA's in the PCB Standards library, are 1:1 scale to the pad size. Since the BGA Solder Mask MUST be pulled back from the BGA pad by a minimum of 0.05mm annular I am considering adding 0.1mm Solder mask oversize to every BGA in the library.

We need to investigate this futher.

[Tom]

Here is an example of the two types of BGA soldermask techniques. See the attached .GIF file that clearly illustrates why we need to pull the solder mask away from the BGA solder pad and "Not Cover" the BGA solder pad like many manufacturers illustrate in their specifications. The ball and the solder paste need to seep over the BGA Solder Pad slightly to improve the electrical contact.

[Tom]

Just attended the IPC Advanced Certification class in Tempe, AZ and they (IPC) are absolutely positive that pulling Solder mask over the BGA Solder Pad is "Not Recommended". The best practice is to pull back the Solder Mask slightly enough so that the Solder Paste runs over the sides of the pad to acheive the best solder joint. They claim that any component manufacturer that states otherwise has not run the proper solderability testing that is required to acheive the highest yield.

See the attached BGA.GIF file that is taken out of the IPC Advanced Study Guide. The picture on the left is the correct image showing a solder mask pullback from the BGA pad. The picture on the right illustres the solder mask over the BGA pad or up against the BGA pad (1:1 scale of pad size or no solder mask annular pullback)

[Tom Frayda]

Just thought I'd add a little more info to the topic.

The general consensus I've seen among BGA design recommendations suggest using Non-Solder Mask Defined (NMSD) pads (where the mask is pulled back from the pads), for the reasons you've cited. Great images there, Tom, by the way.

The other technique is to use Solder Mask Defined (SMD) pads. Here the solderable area of the pad is defined by the aperture of the solder mask opening. The copper land for the pad in this case is larger and the intentionally mask overlaps the land. This is supposed to improve the peel strength of the copper land due to the increased land area and the added strength of the overlapping solder mask, which is said to perhaps help prevent defects due to thermal or mechanical stress, particularly where ceramic BGAs are involved.

However, SMD pads, as you have shown, compromise the solder joint integrity. They also limit the routing and fanout area because of the larger copper land required.

It would seem that NMSD pads are definitely the way to go. Thanks Tom!


+Tom