An Unanswered Question

I've been reading through my Virtual-PCB chat session transcript from yesterday. It was a fun session and I have a much better idea of how the virtual shows work now. I think I may just be getting it.

The chat session had a lot of interesting questions and dialog. I did notice, however, that I missed one question and thus didn't answer it. Oops.

Owen asked if I am of the opinion that all footprints should have rounded pads (probably stencil cutouts too) to help with paste release. Sorry I missed your question.

I'm not of that opinion. There are a lot of factors that come out of stencil decisions. Paste release is one of them. There are others, some more important. For example, the shape of a pad and stencil cut out can either encourage or discourage solder balls. The size of the opening can put too much or too little paste on the pad. Wide open cut-outs over heat slugs can cause float.Bad QFN paste w caption

The pads themselves, should follow the part manufacturers recommendation for shape and size. Most  are rectangular. BGAs have round pads. Unless you have a very good and very specific reason, I would not deviate far from the part manufacturer's recommended footprint.

Some of the factors that influence paste release are the stencil thickness, whether it's polished or not, the angle of the cut, ratio  of thickness to width and paste properties. How long the paste has been exposed to air as well as the room's temperature and humidity can also have an impact. Lot's of permutations.

If you're reading this Owen, Sorry I missed your question in the chat. I hope this answers it for you.

Duane Benson
If it's going to the EU, make sure it's peanut butter free.

Cute Wiring

Yesterday, I wrote about my foibles in ignoring my own advice. As SiliconFarmer pointed outRework 002 cropped over on Twitter, it's not just something you need to do when you're re-purposing a close land pattern. Sometimes even the "correct" pattern can have the wrong drill size or a few mixed up pins.

The bottom line is that if you want to reduce the chance of scrapping some expensive PCBs, or having spots that look like what I did (on the right here), check your land patterns.

I couldn't find my wire-wrap wire late last night, so instead, I used the leads from old thru-hole resistors. It's kind of a mess, but I do like the hatch-markish look that I gave it.

Not to shift any blame off of myself, but I do find it quite annoying when a part falls into such a common standard configuration, as in three-terminal regulator, but the manufacturer picks a different pin-out.

[Note that this is rework I did myself at home. The folks here at Screaming Circuits do  much, much higher quality work.]

Duane Benson
The problem with unwritten rules is that they're unwritten

Lesson Learned... Or Not

MC39100 pin out I've written quite a number of times about the perils of CAD software land patterns. Especially if you don't have an exact match and need to adapt something close.

Recently, I was looking in my Eagle library for a low-drop out regulator, MC39100 is SOT223. It's just a standard, run of the mill 7805 replacement. Nothing special. A million other parts share the same pin-out. Shouldn't be a problem. Shouldn't...

If I were to follow my own advice, it wouldn't have been a problem. But did I follow my own advice? Well, not this part of it. I took for granted that all three terminal regulators follow the 78XX pin-out. Most do, but the LD1117A (below, left) does not. This isn't the first time I've used a non-standard regulator, so I really don't have an excuLD1117A pin outse.

Naturally, I assumed that the pin-out matched what I needed and I didn't hunt down an LD1117A data sheet to verify their pin-out. Well, at least I didn't do so until trying to get my new PCB to power up. Very sad.

So, is there a moral to this story? Probably. Most likely it would be two-fold. One, if you're re-purposing a land pattern from a part that's close, but not exact, double check your work. Get both data sheets out and compare the pin-out.

The second part of the moral is, if you give adice... follow it yourself. Duh.

Duane Benson
Help! I'm blinded by the obvious.

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?

What about the LGA?

I've written a bit about soldermask defined (SMD) vs. non soldermask defined (NSMD) pads for BGAs.

Quick summary: 0.5mm pitch or wider spacing, go with NSMD pads. 0.4mm pitch seem to need SMD pads to prevent bridging (unless the pads are staggered. Then NSMD is fine)

But what about the LGA (Land Grid Array)? It's different due to not having the solder balls. Does that make LGA a difference? According to Freescale and a few other manufacturers, in most cases, you should treat an LGA just like a BGA and use NSMD pads. However, if you need extra strength holding the pad on to the PCB, you may want to consider using SMD pads. As always, consult the data sheet for your specific part for the final word.

Duane Benson
Checkers anyone?

0.4mm Pitch BGA Redux

I've written about it before, and again here.

When dealing with new technology parts, it's really important to look up all of the manufacturer's component information that is available. I'm going to quote from the Texas Instruments document "PCB Design Guidelines for 0.4mm Package-On-Package (PoP) Packages", Section 10 (PDF page 8)

"Industry reliability studies have revealed that NSMD-type pads are highly recommended for most 0.5mm pitch BGA applications. However, there is a problem with this approach at 0.4mm pitch.

Real-world assembly experiments with the BeagleBoard and the OMAP35x EVM revealed a tendency for solder bridging between pads when NSMD were used. There was insufficient solder mask webbing between the pads to ward off bridging. Therefore, a SMD design was used which resulted in much better assembly yields with no solder bridging."

If you are using a 0.4mm pitch BGA with the balls aligned in a grid (as opposed to staggerd), read the design guidlines from the manufacture before laying out the board.

In a presentation about the development of the Beagleboard, Gerald Coley, Beagleboard designer, notes that their first two runs had non soldermask defined pads resulting in a 10% yield. After another run of PCBs where the pads on the PCB were the same size as the pads on the device and the PCB pads were soldermask defined, their yields went to 96%. And verify that your PCB house does in fact follow your instructions. Some will think they know better and will change the mask layout.

If you are still unsure or think your design will have different requirements, call an applications engineer at the component manufacturer and discuss your project and the layout.

Duane Benson
Trust but verify

On Final For Landing on Runway 0805

S part pad shift in oven process Keep out areas can be a problem when adapting a CAD component land pattern, but that's not the only potential problem. Sometimes the part may be close, but the footprint is different enough to cause problems, as in the picture on the right.

You can also run into issues that don't necessarily cause PCB assembly problems, but can be expensive none the less.

Say you are designing with a small microcontroller and the schematic symbol and land pattern don't exist for the one you're using, but something close does. Even though the two parts may look like pin for pin replacements, they may have a few differences.

The PIC family has a number of examples of this. For example, the PIC18F2321 and the PIC18F2455 have enough similarities that they look like pin for pin replacements. However, upon closer inspection, you'll find that RC3 exists on the 18F2321, but doesn't on the 18F2455. SCK/SCL and SDI/SDA are in differnt places on the two processors. You could end up with a bunch of jumpers and a PCB re-spin if you just used one land pattern for the other. It pays to check for those little details.

Duane Benson
Turn left at the big tree, and go until you see the creek.

Keep Out and Keep Off the Grass

The part land patterns in your CAD package parts library should all come with a valid keep-out area defined. That's the theory anyway. However, theory and practice don't always match up so well. I've written a lot about such things as verifying that the actual footprint matches the physical part. That's important. But it's not all that's important.

Caps under BGA Sometimes the footprint will match up just fine, but the body of the part won't. This might be because you're using a different variant of the same part or perhaps a different part altogether that just happens to have the same footprint.

It's common practice to modify an existing library component for a new part, but if you do that, make sure you consider the physical dimensions of the part body too. Sometimes you can get away with the keep-out area being different, but as shown in this image, not always.

Duane Benson
Keep off my lawn, ya young whippersnapper!

Monsters Under the Bed

TO-263 land with mistakes Monsters, metaphorically speaking, that is. Take a look at this little land pattern for a TO-263 part. Can you tell me the two main things wrong with this land pattern?

I'll give you a hint. One of the problems is an absolute no-no. The other one could be justified with a low-current application. But then, wouldn't you use a smaller package?


Duane Benson
Green Grow the Traces Ho

Narcissistic Parts

Maybe not completely narcissistic, but at least self-centered. Or, self-centering. Okay, are you lost now? Am I making any sense at all? Well, I'm going to say that it doesn't matter, because the world-revolves around me.

But what I am talking about is parts that will more or less center themselves during the reflow process. Some parts like BGAs and QFNs tend to follow the surface tension of the melted solder and tweak themselves into a more centered position on the land. That's a good thing.

Ground pad pulling part It's not always a good thing though. Sometimes that same surface tension action can work against you. Take this TO-263 part on the left. When it was placed on the land, before reflow, the leads were centered right in their pads like they should be. The big land for the thermal pad is set up a little too high though and once melted, the surface tension from the big thermal pad sucked the part up, nearly dragging it off of the lands for the leads. Bummer days. (Here's another example)

You probably shouldn't leave the part like this, so here's a few suggestions:

You could make the thermal pad smaller so that when the metal tab of the part is centered, the leads will be too. Cooling needs might dictate that you don't reduce the size of the pad though. If that's the case, you could make the bad bigger by extending it down toward the leads, again so the leads will be centered when the body of the part is. You could also mask off the top part of the pad, or put a thin strip of mask as a solder dam. What you're doing is making sure that if and when surface tension moves the part, the leads will end up where they are supposed to.

Duane Benson
It is all about me, you know