Screaming Circuits: Tips and tools


A lot of small quantity PCBs come individually routed these days, but when they get too small or come in larger quantities, panels can be very nice to have. When you have your PCBs panelized, what's your preferred method? And why?

We get questions about this reasonably often: "What's the best way to panelize my boards?" For our shop, we have some guidelines on how to go about it (make sure to follow the specific guidelines from whatever manufacturer is assembling your boards), but the guidelines don't specify whether you should use V-score or tab routed. That's a decision left to you.

V-score section What if you don't know? Well, it depends then, but you can easily eliminate a few options. For example, if you have curves in your board outline, you can't V-score. V-scoring only works in straight lines. With curves or odd shapes, you have to use tab-routed. If your outline is a pure rectangle, V-scoring tends to require less board-edgBoth tab and 
v-scoree so you can get a bit more out of your PCB real estate. But it's more difficult to deal with on very thin boards and V-scoring leaves a rougher edge after snapping the boards apart.

Two of the key disadvantages of tab-routing are the greater waste area and the nubs that stick out after separating the boards. You can leave the nubs, sand them down or use a clean-up router.

Here's my take on it: A) If it truly doesn't matter, use whichever method is less expensive or that you think looks prettier. B) If you have curves or other odd shapes, you'll probably need to go with tab-routed. C) If your boards are rectangles and you can deal with the less-smooth board edge, go for the V-score.

Duane Benson
Tab. Not Diet Coke.

Thermal Mass Follow Up

RoHS has been with the electronics manufacturing world for quite a while now but there is still a lot of issues and uncertainty associated with it. As I wrote not long ago, even parts that are supposedly compliant can in some cases not cut it.

Taylor asked in the comments section of that post: "Have you noticed any pattern in capacitor manufacturersClose caps 3 exhibiting this problem? How can make sure to spec a capacitor that is more robust?"

Close caps 1 I can't say that I've seen a real consistent pattern with components from different manufacturers here. It's a case where the design engineer may have to compare the exact thermal specs from different components' data sheets and throw in a good measure of intuition and judgment as well.

In some cases, you might be able to replace a couple of capacitors with a single of a larger value, but in general, if you need multiples, combining them won't do. There are certainly good reasons to parallel up capacitors. You may need a few of different values to cover different frequencies. You may have a clearance issue and not have enough height for a taller cap. Or you may need to keep the ESR (Effective Series Resistance) down. Whatever the reason, if you need a number of caps close together, and they are big SMT electrolytics, you could be setting yourself up for this problem.

Close caps 2 Image A illustrates the issue found in that earlier post. The thermal mass of all of those big metal can caps can slow the solder melt. The most vulnerable pads are the two inside pads for C3 and C4. Keep the heat up long enough to fully melt the solder on all pads and you may destroy the caps, or other components.

You could just spread the two rows apart a bit like in illustration B. This might be enough to allow all pads to solder well or, if nothing else, it would give you enough room to touch up with a soldering iron.

Probably the most common solution though is to take the approach used in illustration C. Just put all the caps in a row so none of the pads are vulnerable.

If you need a compact layout like A, you'll just need to spend some extra time with datasheets to find a specific cap with a bit of extra RoHS temperature margin. Look at the maximum solder temp, the maximum dwell time and the profile curve if available. Don't forget to check your other components too to make sure that the extra reflow time wont harm them either.

Duane Benson

More Thermal Mass Issues

Yesterday I wrote about some thermal mass related traps. Here's another one we see now and then.

Over heated caps

The top image shows good flat-topped caps. The bottom and inset has overheated bulged and damaged caps. These caps are RoHS compliant - supposedly. Their data sheet calls them out as RoHS compliant and their temperature specs and recommended reflow profiles indicate RoHS compliance. So what happened?

Well, they are compliant pretty much only in singles. A single of these caps will solder up fine and not be damaged. However, put four in close proximity like this and the solder paste on the inside pads will not melt at the recommended profile. They need a bit more heat because the thermal mass of the four parts close together sinks heat away from the inside solder pads. In the end, we hand soldered these specific parts to solve the problem, but for production, either a more thermally robust part would be needed or the part spacing would need to be changed to compensate for the combined thermal mass.

Duane Benson
"Hot" is a relative term

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