Screaming Circuits: November 2007

Surface Mount EMI Gaskets

Here's an interesting board.

Emi_sponges_on_board_edgeEMI gaskets have been around for a long time. Some are foam. Some are springy metal and some are wire braid. They all do the same things though - create a seal between your EMI source and your EMI shielding. We ran this board recently that uses a foam gasket from Gore Industries. It's a pretty cool product in that it can be run through our SMT machines just like any other surface mount part. No secondary or hand operations are required.

While I have the picture of the board up, there are two things I'd like to point out. (Always have to be the critic. Right?)

Emi_sponges_top_view_2 [Click the picture for a closer view] First, at the label "A", there is a part that looks to require a specific orientation. It has four leads and a directional marker on the part. You will note, however, that the board doesn't have a pin on or polarity indicator any where. We got it right - probably had an assembly drawing or illustration, but a pin one mark on the PCB would be a much more reliable method.

Second, at the label "B", you will notice that one of the pads for the little cap is in the middle of a real thick trace. The other pad has a very tiny trace connected to it. There may have been an impedance reason for doing this. I don't specifically know, but if not, you should avoid a layout like that with small parts. The thicker trace on one side can act like a heat sink and slow the paste melt on that side. Then when the solder paste on the other side melts first, surface tension can cause the part to pop up like a tombstone.

Duane Benson
EMI is mighty fine

A Little Pad In That Via

Here's an interesting via-in-pad situation we ran across a while ago. I'm not sure what the chip is. Probably a processor or an FPGA that generates a bit of heat.

The intention with the layout was on the right track. However, the implementation wasn't really workable. All of those big vias were put there to sink heat away from the thermal pad on the bottom of the chip. The vias being so large, heat would be removed by air convection as well as conduction through the via walls. The thought is good.


In practice though, there are a couple of big problems with this approach. First, the pad on the PCB is much larger than the pad on the chip and the extra area is not masked. Even without the vias, that could make for more difficult solder control. The biggest problem is simply the large open vias. It really isn't possible to solder such a layout with standard surface mount process. Since this is a prototype, we found a way to make it work, but for volume manufacturing, as well as for cost reduction in the prototype, a different approach is needed.


In the second image here, we've simulated what a good workable footprint could look like. This isn't the only possible way to do it, but it would work well. Here, the exposed pad matches the size of the heat slug on the chip. The rest of the pad is still there for thermal conduction but it is masked off. There are a generous number of thermal vias in the masked area and a few capped vias in the solder area. Even better would be to plug and copper-plate over the vias in the solder area, but this way works too and is less expensive at the board fab house.

Duane Benson
Flying spaghetti monster says what?

Copper and Tombstoning

Earlier this week, I wrote about the effect soldermask can have on tombstoning and I referred back to two older posts on the subject of tombstoning. I also wanted to refer back to a third tombstoning-related post that talked about the effect that your copper can have on tombstoning, but I couldn't find the post. Well, apparently, I never actually wrote that post. I meant to but forgot and moved on to other subjects.

Any, way the point I wanted to reference related to the heat-sinking characteristic of copper. With small parts, uneven heating can lead to tombstoning. If one side of the solder paste melts before the other, Tombstoning_uneven_route the surface tension on the melted side can pull the part up.

In the first case illustrated here, (click image to enlarge) one side of the part has a small trace going to it. The other pad has a much wider trace. The eider trace can act as a heat sink and slow the melt of the paste on that side, causing the tombstoning.

Tombstoning_inner_layerIn our second illustration, (click image to enlarge) an inner copper layer goes under one pad but not the other. As with the wide trace, the inner layer may sink heat away from that layer and keep the paste from melting at the same time on both sides.

It may not seem like much, but an uneven melt of just a very short time span can lead to tombstoning. That makes it a good practice, especially with small parts like 0402 and 0201 passives, to consider the thermal characteristics of your layout.

Duane Benson
Oh! ye'll take the high road and
I'll take the low road...

Soldermask and Tombstoning

Tombstoning isn't too much of a problem for us or most of our customers theses days, but it still does happen for a variety of reasons. For example:

The most common cause these days seems to be solder mask related.


We have found that sometimes, if the solder mask is too thick and rises up above the level of the solder paste deposits, very small parts (0201 and 0402) are more susceptible to tombstoning.

In example A, the solder mask is thin enough so the part can rest on the past and will reflow properly. In example B, the part may rest up on the solder mask and not fully contact the solder paste on one or the other side. This can cause an open or lead to tombstoning - especially if the mask has bumps or variations in the thickness.

Good mask registration will help. Using a board vendor that has tight tolerances and delivers a thin flat mask surface will help. In some cases, with the smallest parts, you may want to keep the soldermask off the pads - use non solder mask defined (NSMD) pads.

Duane Benson
Carry on my wayward capacitor

Holiday Closure

Turkey_2We will be closed on November 22rd and 23th, 2007. This means that those days won't be counted toward your turn times. For example, if you have asked for a 48 hour turn time and we receive your kit on the afternoon of the 21st, your 48 hour clock will start on Monday, the 26 .

We apologize for any inconvenience and wish you a happy holiday.

Duane Benson
Can anyone tell me the proper reflow profile for a 20 lb turkey?

Passives and Via In Pad

Small_fillet_passive_via_in_padAre you tired of this topic yet? Myself, I'm a bit scatterbrained so I can pretty much talk about the same thing forever. And, I can repeat myself and not even feeling like I'm being redundant or repeating myself. I'm not sure what that little dip into my personal philosophy has to do with the trials of one tasked with a complex layout, but I certainlySkewed_passive_via_in_pad_2 know what via in pad has to do with it.

Most of our via-in-pad articles relate to QFNs and BGA type devices, but via-in-pad can also impact passives. It can cause tombstoning, part misalignment and open solder joints. Here's a couple of examples where the open via didn't cause an electrical open - both have good electrical connection, for now - but there is almost no fillet and very little solder under the part. These will work at the initial turn-on but after a few thermal cycles and maybe some vibration or rough handling, they are very susceptible to cracks in the solder joint on the via side.

If there are other parts really close by, the crooked part causes a shorting risk as well. A misalignment like that happens for the same reason that tombstoning can: Capillary action from the via sucks solder away from the pad and The via sinks heat away so the solder on the other pad melts first. Then the surface tension of the liquid solder can pop up or move the part around like this.

Duane Benson
305 down, 60 to go...

« October 2007 | Main | December 2007 »