Screaming Circuits: Tips and tools


Thermal Mass

I mentioned thermal mass in a recent post and was thinking over my oatmeal that its a subject deserving of more attention. That's more attention to thermal mass, not to oatmeal. Although, oatmeal is a pretty healthy food so it probably deserves more attention then it gets these days.

When most people think of thermal issues, the considerations tend to be around operating conditions. Will the part generate too much heat? Will there be enough airflow or is there enough surrounding material for adequate conduction cooling? All of those are pretty important - especially with the obvious like fast processors and big honking power components. But there are a lot of thermal issues related to manufacturing that have to be considered as well.

Reflow soldering is supposed to gradually and evenly warm the PCB and parts up. Then, the temperature will spike up just high enough and long enough to melt all of the solder before dropping again. This is were thermal mass trickery comes in to play.

If you have a tiny passive part and one pad has a lot more copper then the other - it can even be a problem Two part tombstone even if it's an inner layer with more copper under one pad then the other - that extra thermal mass can delay the solder melt on that side of the part slightly. That delay in melting can cause the surface tension on the side that did melt to pop the part up like a tombstone. Placing a very large component too close to one side of a very small part can also cause the same problem.

If you have really tiny parts, give your layout (inner and outer layers both) and placement a scan to make sure you haven't inadvertently created a heat sink on one pad and not the other.

Duane Benson
Quick. Call Wilford Brimley

Toyota is as Toyota does

Everyone else seems to be writing about Toyota sudden acceleration problems, so I should probably do that too.

Or should I? Personally, I have absolutely no solid information about what's going on with Toyota cars. There's an awful lot written, much of if by people that also don't have any real information on the subject. Here's what I do know though:

  • Some people (some with actual knowledge and some without) are speculating that electronics might have something to do with the problems.

That's about all I know relative to the specific concerns. On the soft side, I do know that people tend to pick on the big guy. Funny how none of this was big news until Toyota became the #1 car maker in the world. Coincidence? Maybe. Maybe not. I also know that in any system there are gobs of places where LED via-in-padissues can lead to failures. Of course, to counter that, I know that good, well thought out design - both in the hardware and the software, can produce a quality product that will keep working. In summary, I really don'tSilk on pad know anything about the Toyota issues.

However, any time some sort of actual or potential technical problem makes big news, it's not a bad idea for those that design and build things to take a step back and evaluate our design practices. I've got software in my past, so I'd have to suggest a good solid code review, if you don't already do one, but today, I'm talking about hardware so I'll sample just a few things to double check.

  • Those pesky land patterns: Does the land pattern fit the part? Will the copper area and stencil opening allow for a good solid IPC-passing solder joint? It's so common (as you well know if you read here regularly) to re use or create new CAD part foot prints. Make sure the foot print, stencil, mask and silk layers fit properly.
  • Vias in pads: Plug them and plate over them when using small parts. If the solder surface is big enough, like with a power component, you might be able to just cap them, but don't leave the vias open. In some cases, you may be able to leave very tiny vias open on thermal pads, but it's best never to.
  • Thermal mass: This is important both for operation and for assembly. If you've got components that sink and/or generate lots of heat, make sure there is enough air flow to cool them during operation and make sure that the assembly house can build it. Put a couple of high thermal mass parts too close together and an otherwise perfect PCB assembly may end up with some cold solder joints or damaged components that later come back to bite you or your customers.

There are lot's of other things to check out too, but those three are just some of the more common traps to keep tabs on.

Duane Benson
I don't have a Toy Yoda. If I did, I'd sell in on eBay.

Ambiguous PCB Markings

Which ref for which partHere's a little issue we run into now and then. Which reference designator goes with which part? Quick. I need to know. Now. Now. Now!

It's less of an issue with SMT parts because we machine place them and use your centroid file to do the programming. Still though, It's always good to have things marked clearly in case rework is needed and for visual inspection.

For thru-hole, though, it is definitely an issue because a real human being is putting the parts in and the visual markings are the programming for the human type person.

For best results, take a little extra time and make sure all of your ref designators are clearly associated with the correct part. It's also always a good idea, when possible, to have all the designators in the same position relative to their part. Consistency is a good thing here. Consistency is a good thing with mashed potatoes too. Who likes lumpy mashed potatoes?

Duane Benson
You say poe-ta-toe, I say ugly brown tuber

Inverted QFN Land Pattern

Have you ever experienced the heartbreak of inverted land pattern? It's not supposed to happen, but every now Inverted QFN land pattern 2and then, it does. Maybe something happened when creating a custom footprint. Maybe, somehow it got inverted in the CAD software and then placed on the wrong surface layer.

Maybe it was a subliminal attempt to make up for those giant open vias in the thermal pad. Who knows. But, it happened, so now what?

You could re-spin the whole board. Ugh. That's, like, wasteful and stuff. Certainly, if this is a production build, you'll have to re-spin. For some prototype applications - like if it's a high frequency or RF thingy, you may very well have to get a new set of PCBs fabbed up too.Inverted QFN land pattern

But, sometimes in the prototype world, you may be able to salvage the board run. We used to do stuff like this all the time with  thru-hole parts - need an extra chip, just dead bug hang it on up there. 

Flip the chip over and use some small gauge wire - maybe wire-wrap wire - and hand wire to the upside down chip. Gluing it down first may be helpful. Just keep in mind that since the thermal pad isn't soldered to the board, you will lose some of your thermal performance. Maybe solder a small heat sink on it or something. And don't forget to wire that pad to ground too (if it's supposed to be grounded).

Duane Benson
Just put it on the seventh surface of your tesseract and it will fit right.

You got C in my L. No, you got L in my C

Parts too close

Just another tale of a poor little capacitor feeling lonely and trying look up to a big inductor for advice and guidance. Sadly, Henry, the inductor rebuffed the little uf with nary a word and kept his emf to himself.

Duane Benson
Ell Sea can you say the donzer lelight

Via in Pad with Passive Components

Most of the via-in-pad writing I do concerns BGAs and QFNs. I do cover other parts from time to time, but the subject seems to come up most often with those packages. It is an important subject with passives too though. If you need to make your board smaller, putting vias in the pads of all of your passives may seem like a viable option to gain a lot of space. If you fill and plate over the vias, then, yes. It's a good plan. If you leave the vias open, then no. It's not.

Here are some via-in-pad guidelines:

Part type
open viaSolder mask
capped via
6mil or smaller
open via
filled and
plated over
BGA and LGA land padsBadBadBadGood
QFN, TO-(power part) thermal padsBadAcceptableMaybeGood
QFN signal padsBadBadBadGood
Passive padsBadBadBadGood

You can probably see a somewhat common theme in the table above.

Move via to the left Silver QFN vias vAll of these pictures show bad stuff. These are from the "don't ever do this" camp. Open vias on passive parts can lead to 9x13 via in pad BGA land tombstoning, poor mechanical connections, solder blobs on the back side of the board and crooked parts. Open vias on BGAs can also lead to the solder ball being sucked off of the the BGA. Bummer dude.

If you do use solder mask capped vias in a thermal pad, most manufacturers recommend the via cap be about 100 microns bigger then the via. This prior post here shows a decent example of using solder mask caps in the center thermal pad of a QFN (the rules from QFPs and DFNs are the same as for QFNs). And, I'm calling it a thermal pad in the center of the QFN, but the rules still apply of the pad is just for grounding and not for cooling.

Duane Benson
Where are we going? Planet ten
When are we leaving? Real soon


 

Solder Paste Stencil Opening

Stencil openings too bigHere's a case of "close, but no cigar" with the stencil opening. The pads are, in fact, covered by the openings, but as you can see, the openings are too big.

This stencil would end up laying way too much paste down. Some of it would be on the solder mask which might bubble up and turn into solder balls. All in all, the use of this stencil might just lead to something of a gloppy mess.

When you're making your paste layer in the library component (presumably, this was custom made), it's sometimes appropriate to make the paste opening the same size as the pad and it's sometimes appropriate to make the opening smaller, but it's never appropriate to make the opening bigger then the pad size.

After writing this, I for some reason got curious as to the origin of the phrase: "close, but no cigar." I know it's been around a long time, but I couldn't come up with any plausible meaning for it. Then I remembered this thing called the Internet, so I looked it up. According to a couple of different sites, carnival booths, like the big hammer, would give out cigars as prizes so if you almost made it, the Carney, would say "close, but no cigar." Huh. Interesting, but much less interesting then I had expected.

Duane Benson
Sorry. We don't give out cigars if your stencil is good

And, Another Thing...

I got a couple of pretty thorough comments on my copper pour post over in the Circuits Assembly blog where it's also posted.

David le Comte wrote:

"...On two layer boards (with 5V CMOS logic in particular) it is very difficult to pass CISP-22 EMC tests without a well grounded flood plane.

In the 1980s it became a requirement for more and more categories of electronic equipment to be tested for EMC compliance.

From first hand experience, I have seen how just adding a flood plane to two-layer boards can reduce EMC by 20dB. (We had to revise existing boards to pass EMC tests during the late 80s and 90s)..." (See his entire comment on the Circuits Assembly blog link above)

That brings up a very good point. EMI. In the prototype/experimental world and the hobby world, there are so many cases where EMI isn't too much of an issue. We don't always think about it. If your project is going into a consumer or business consumer product, no questions, though, EMI is a big consideration. As David indicates, a grounded pour or plane can go a long ways toward keeping stray interference down.

I wonder if an Arduino could pass any EMI standards. Has anyone run it through a lab? Maybe with some good shielding. I bet the "Knight Rider" teeth I made for my pumpkin this Halloween (with a point to point wired PIC16F819) just radiates all over the place.

Duane Benson
Pore, pour, pitiful me

Pour Or Not - Just What Is My Opinion?

I posed a question about using copper pours (AKA flood) a not long ago. The premise was a simple microcontroller board with a 20MHz clock and no special requirements.

Cooper pour exampleI had a couple of different comments on the post with some very good insight. Myself, I generally don't use copper pours. My only reason is that I think it usually looks better without. Although, I do like the look of the cross-hatch pour on the Arduino. A well done flood can be pretty cool, but still my inclination is to only use it if it's needed. If it's a shop doing the PCB, the metal will be recovered and recycled, so the conservationist in me is pleased.

If it's a home etched deal, then a pour is probably a better idea because it will reduce the amount of etchant needed. Although you do need to be careful to keep plenty of space between things to prevent solder bridges. Solder bridging isn't such a big deal on a PCB with a good solder mask, but it certainly is on a board with no mask or thin mask.

If there is a good reason, I will. Like a high-current motor driver - I use the pour to keep the current capacity up and the kelvons mellow. Heat sinking is a good reason for a pour. Hi speed stuff usually benefits from a flooded plane of some sort too and in four-layer boards, using the inner planes for power and or ground is nice and convenient. But you all know that. I'm just rambling now.

Duane Benson
Does high speed stuff on a flooded plane require a speed boat?
Will too much heat sink it?

Diode Silk Screen Markings

It still happens. In fact, it just happened last night. We had a PCB with plus (+) mark to indicate the polarity of a diode. Unfortunately, that doesn't tell us which way to put the diode. (Read why here).

Schottky top You just can't always tell. If it's a barrier diode or a zener, the cathode might very well be the positive side. Or, it could be the negative side. An LED will usually have the anode positive, but again, there may be a few scenarios where it's not. The bottom line is that a plus (+) or minus (-) sign doesn't give us enough information to orient the diode.

We prefer that you use the actual diode symbol, or an industry standard anode or cathode indicator. "A" orGood markation "C" for anode or cathode can also work. Just make sure you also put the reference designator (D1, D2...) so we know it's not a capacitor.

In the job last night, the build instructions were conflicting so we called and with the help of the designer, figured it all out, but it's always best to do it right the first time. So be clear with your silk screen, the PCB you save may be your own.

Duane Benson
Spider or worm?