BGA Woes

Quite a few of the new chips I see coming out stick to the BGA or QFN form-factor. Sometimes they'll be referred to as WSP (wafer scale package) or CSP (chip scale package), but those are still just little BGAs. Some do show up in larger packages, but many of the really new designs seem to stick to these form-factors.

A few years back, we tended to see a lot of design problems related to regular, big BGAs (0.8mm or greater pitch). Things like black pad,  microvoids and via in pad cropped up to cause proto-headaches. While those problems still show up from time to time, they have become much less frequent. No, we're seeing issues with the tiny ones - 0.5mm and 0.4mm BGAs, CSPs and WSPs.

With a big BGA, you can route to vias in between the pads. That's easy. With the small ones, especially 0.4mm, you can't. You have to put the vias in the pads. Of course, you have to fill and plate over the vias. Big BGAs tend to prefer non-soldermask defined pads (NSMD) while some of the 0.4mm BGAs require soldermask-defined (SMD) pads. A really flat surface is more important for the tiny parts too. Don't fear extra small parts, but you may need to do a bit more homework and relearn a few old rules-of-thumb.

Duane Benson
I'm solderin, I'm solderin, I'm solderin for you

A Bit More On the LGA

After my last post about LGA land patterns, I received a couple of questions asking for more detail in a few areas.

"The LinearTech  LGA apnote (LTM46xx series) shows planes on the mounting layer interconnecting pads that are solder mask defined. This is supposed to be for heat dissipation. Will smaller copper defined pads and vias to full internal copper ground and power planes provide adequate cooling?

What about using LGAs on the same layer as BGAs? BGAs have copper defined pads? We've been sending 1:1 soldermask gerbers to the fab house so they can adjust per their process. Can this be done selectively so the SMD LGA pads don't grow bigger? What kind of Fab Note should be in the "Readme" file?

Also, please warn LGA users to be careful using wizards (eg Pads Layout) to generate the pad numbering. Linear Tech's LGA does NOT follow the standard BGA alpha numeric numbering. I don't know about other LGA mfgrs numbering systems but ... Double check the pad numbering and avoid this nasty snake bite!"

First, as far as cooling goes, the answer, unfortunately is "it depends on how closely to the limits you are driving to part." You will get best results with more surface copper. That being said, you can use vias to internal and back-side planes to increase heat dissipation. Ideally, you would have Lot's of surface copper and vias to the internal and back side planes, but that's not always possible. The vias that are not under the LGA pads can be left open. Any vias in an area to be soldered must not be left open. Ideally, you would have them filled with a thermally conductive material and plated over. You do have some flexibility to reduce the surface copper and replace it with vias to other planes, but ultimately, the final answer will only come from your design testing.

You can have NSMD and SMD pads on the same PCB. How to do it is the big question here. Many fab shops will make their own decision on what is "best" for your PCB in this regard. I would speak with the board house and get their recommendations on how best to specify what you need in terms of NSMD and SMD mixed. You'll probably have to follow a slightly different procedure for each different fab shop.

I would double echo the comment about using caution when using wizards to create a land pattern. Not all manufacturers follow the same numbering scheme. You could get bitten badly with this one.

Duane Benson
Who was that soldermask defined man?

Hand To Machine

It's getting very difficult to hand solder many parts these days. Some people give it a try, but in general, if you're dealing with the really tiny parts or leadless parts, it's just not possible, or at least not  practical.

Sometimes a designer will start out with the idea of hand soldering the board up and then either decide against it when first looking at the raw PCB, or will build one and then decide that it's too much work. That's not a bad thing. You can get more reliable assembly and it keeps me employed. But there are times when a layout designed with hand assembly in mind does not work for machine assembly.

Case in point, this image. Now there are two things wrong here. The first is that the land pattern is for  a smaller part than the actual component. Let's pretend that problem doesn't exist. The other problem is that big via hole in the middle of the pad. When hand soldering parts with a solder pad underneath, like QFNs or QFPs, folks will often put a large hole there. They'll solder the outside connections first. Then, turn the PCB over and stick a soldering iron and some solder in that big via to solder up the pad.

That works more or less for hand soldering, but it's a really bad thing to have a big open via like that when machine assembling parts. The solder will flow down and out the other side. You'll get a mess on the bottom of the PCB and you may get little or no solder on the pad.

So, the moral of this story is that if you've designed your PCB for hand soldering and later send it out for automated assembly, go through the layout and make sure you remove things put in there for hand soldering that aren't conducive to reliable machine assembly.

Duane Benson
Don't fall in...

Via Caps

The best way of dealing with via-in-pad requirements is to have the vias filled and plated over at the board house. There can still be some issues with that technique, but if done right, is very reliable and the best way to go. But, what do you do for a Klondike bar? I mean what do you do if you can't afford to fill and plate over your vias, or don't have the time? Well, if your vias are in a BGA pad and you don't want to have them filled and plated over, than you can just go back to the drawing board because your board most likely won't work. There may be some secret, prototype-only things that your assembly house can do, but avoid it at all costs.

If your vias are under a QFN or SOT-23 or something bigger like that, you have more options. Don't leave them open. Worms will use the open vias as homes. You can usually use soldermask to cap your vias in cases like this.

C is not an option. A and B can work. D can work also, but should be your last choice. With the tight masking like in A, most manufacturers recommend that the soldermask cap be about 100 to 125 micron wider than the diameter of the via. B is self evident - just make it bigger.

The pitfalls with D are that solder will still get sucked down into the via which can lead to excess voiding. Or, the via cap could pop open which results in effectively a C. With all soldermask via caps, top ot bottom, you need to check carefully to ensure that the soldermask gives a complete seal. And there is always a risk of the cap breaking. Ugh. Now do you see why everyone recommends filling and plating?

Duane Benson
The worms crawl in
The worms crawl out
The worms play pinochle on your snout

Little Chippy Challenges

And in terms of "Chippy", in this context, I'm referring to chip-caps and any other tiny little two-connector components. When considering surface mount, most people think of the many-connector parts, like BGAs and QFNs as the challenging components. That's mostly true. However, the little passives can be big bears too if not treated properly.

You can have tombstoning problems. This can be caused by unequal sized pads, unequal sized traces going to the pads or inequality in copper plane in a different layer. A big part on one side can cause tombstoning too - the big part's thermal mass may slow the solder paste melt on one side of the part, leading to  tombstoning.

Via-in-pad is still a problem too. Open vias can lead to unreliable connections, tombstoning or crooked  parts.

Solder mask can cause problems too. Too thick a solder mask can prevent the part from reaching the solder and can cause tombstoning. That thick solder mask can also interfere with out-gassing in the reflow oven which can cause solder ball splatter. (A = okay, B = at risk if mask is too thick).

Duane Benson
It just goes to show you...
It's always something.

PCB Planarity, Not Polarity

Via-in-pad can ruin a manufacturer's whole day. Or, if properly done, can go completely unnoticed. There are a number of ways to properly put a via in a pad but the best is to have it filled and plated over at the board fab house.

If you do that, check with them on their planarity standards. If they don't hold tight, you can end up with a  dip or a bump where the via is. Neither of those are as big a  problem as an open via, but they can still lead to some difficulties.

Speaking of bumps, the old standby, HASL, generally leaves bumps on the pads too. And, across the span of a BGA, the bumps can vary in size and shape. That's not such a good thing either. If you're designing with a fine-pitch BGA, you might want to consider a flatter surface such as ENIG or Immersion Silver.

Duane Benson
Fight Uni

Random Via-in-Pad Myth #7

Myth #7: In regards to via-in-pad, all PCB finishes are the same 

Well, it might seem so, but let's look a little closer. No. Not that close. Back the camera up a bit. 

Here's a good example: In some cases, it's okay to seal off the via with soldermask on the opposite side of the board. It's not the optimal way to do it, but when the geometries aren't that small, it can work. It needs to be a part where voiding isn't an issue, because the solder may still go down the via and cause some of those voids. "Void" may be accepted in C code, but it's usually bad form in a PCB.

Getting back to the subject... Immersion silver gives a nice smooth surface. It's fairly easy to solder and provided the boards are used promptly or stored properly, it's a good RoHS choice.

But, it's not a good choice for a situation where you cap a via with soldermask on the underside of the PCB. The immersion silver finish will likely out-gas a bit and when contained, as in the sealed off space between the solder on the top and the soldermask on the bottom, that outgassing can be corrosive and lead to reliability issues sometime during the life of the product. So if you do need to have vias that are capped on the bottom side, you should consider a surface finish other than immersion silver.

Duane Benson
No more silver on Walden Pond

Random Via-in-Pad Myth #3

Myth #3: It’s okay to put vias in BGA pads because the extra solder (the solder ball) on a BGA will prevent any problems

Here's an example of a via in pad situation we don't like; A large number of vias in the BGA land pads. They're pretty big via holes too. The primary reason we don't want to see vias in pads is that when left open, those via holes act like little capillary straws and suck solder off of the pad. A couple of undesirable events can happen depending on the method used during board fab.

If your vias are left open, solder will tend to wick down into the via hole. The larger the diameter, the worse the wicking problem can be. You might end up without enough solder left to secure the component, or even a solder bump on the bottom side of the board which could interfere with other components or lead to shorts.

The extra solder in the BGA ball can just make a bigger mess on the back side of the board. And the extra space that BGAs have between the component and the PCB make opens even more likely. BGAs are more susceptible to this problem. Not less.

Some people will try to use soldermask to cap the bottom side of the via. However, the solder ball can still be wicked down into the via, leaving an open. Or the soldermask cap map pop off due to thermal expansion or out-gassing, leading to a purely open via. Internal air bubbles can migrate up, leading to voids in your solder joint.

Duane Benson
Burma Shave

Re-runs

I've been pretty occupied with the upcoming Embedded Systems Conference in Boston. The exhibition is next week on Tuesday, the 21st and Wednesday the 22nd. Screaming Circuits will be in booth 809. Stop by if you happen to be at the show.

In any case, I've been pretty much wrapped up in show preparation so I haven't had much time for original writing here. That being the case, I'm going to play an old TV sit-com trick and just select some old, but good, content to re-run.

• Here's one about an, apparently controversial, usage for via-in-pad.
• Some handy tips related to using multiple thermally-large components.
• What to do if your QFN footprint somehow gets inverted and mirrored.

And, there you go.

Duane Benson
Hide Wally Bee. Andre is back and he's got a fly swatter

Via-In-Paste

I've heard of vias in pads, but vias in paste aren't so common. Here's a QFP footprint with a lot of thermal vias in the center pad area. I'm guessing all of those vias are necessary for heat removal, but they sure aren't friendly to solder paste as created.

Further, the solder paste stencil had good intentions too, but ended up inverted in practice. It's good to keep paste off the vias. Even inverted though, I'm not sure how the stencil would have worked. You can't have dots of stainless steel just floating out there. The vias should be capped, or better yet, filled and plated over. The proper way to create the stencil layer would be with a cross hatch as shown in the third image.

Capping (also called tenting) vias with solder mask used to be a pretty common practice. You'd put solder mask over the via out to about 100 microns bigger than the via on the component side. Some people would put the cap on the back side, but that still leaves a lot of volume for solder to wick down into.

The capping with mask practice is kind of falling out of favor these days. For one, if the mask is too thick, it can end up lifting the part up a bit. More likely though, the caps can break, leaving an open hole for solder mask to wick down.

The optimal method is to have the vias filled and plated over at the board house. There are some thermally conductive materials that do just about as good at heat transfer as would the open via.

Duane Benson
Solder paste is people! It's people!