Tag Archives: NSMD

Let’s Talk about HAL – And Another Thing

Posted on by

A few days ago, I wrote about HASL PC board surfaces, explaining that it’s not an appropriate choice for small parts.

Look at the same PCB image I used the other day. You might not recognize it because before it was on the right, and today it’s on the left. Getting past the fact that I just insulted everyone’s intelligence, there is something else about this board that we don’t recommend.

I’ll give you 30 seconds to figure it out. I don’t have a stopwatch, so the 30 seconds is on the honor system.

This is a land for a 0.5mm pitch BGA. As I wrote before, HASL is not the right choice for BGAs, especially for those of the smaller pitch variety. The other problem with this board is in the pad layout.

These are solder mask defined (SMD) pads – the solder mask covers the outer part of the pad, so the solderable copper surface is determined by the size of the opening in solder mask, not by the area of the copper pad.

For BGAs 0.5 mm pitch and larger, we (and pretty much everyone else) recommend non-solder mask defined (NSMD). With a NSMD pad, the solder mask opening is larger than the pad. This leaves more copper area to adhere to, including the sides of the copper pad. It tends to be much more reliable.

The image to the right illustrates the difference. 

The left-most pad in the image illustrates an SMD pad, while on the right is an NSMD pad. The NSMD pad leaves a lot more surface area of the copper pad for the solder ball to grip on, including the sides.

BGAs with 0.4mm pitches might need either SMD or NSMD pads, depending on a number of circumstances. Read this blog information for a bit more on 0.4mm. When in doubt, look in the back of the datasheet.

Duane Benson
Question for physicists and mathematicians:
Should the last recursion in the Mandelbrot set land on Plank’s constant?
Show your work.

http://blog.screamingcircuits.com

 

A Bit More On the LGA

Posted on by

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 (e.g., 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 manufacturers’ 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 said, you can use vias to internal and back-side planes to increase heat dissipation. Ideally, you would have lots 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 its 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?

http://blog.screamingcircuits.com/