Screaming Circuits: Tips and tools

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?

Hmmm. Black Pad Does Happen On Other Parts Too.

Well, lookie here. Just the other day, I wrote about black pad happening on gull-wing partsQFP fillet bp. I also wrote a while back about the footprint on gull-wing parts - the fillet under the part is even more important to mechanical strength then is the visible fillet on the outside of the part. This morning, I was browsing back through some of my old parts images and I accidentally gave this one a good bump. And with a spot of ironic annoyance, a couple of the leads popped loose due to what appears to be black-pad.

I thought I was being careful with my nickle when I made this illustration earlier this month, but I must have let some contamination through. Maybe I was eating cookies at my desk between the nickle step and the gold step. How rude.

Duane Benson
If they were chocolate chip, then it was worth it

To Pour, Or Not To Pour. That Is The Question

Pcb w o pour Pcb w pourI know there are plenty of times when a copper-pour ground or power plane is a good idea, sometimes even a requirement. But, is it always so? Take a simple embedded microcontroller board. It has a 20MHz clock speed. Nothing too dramatic. No big power drains anywhere. Just milliamps going here and there.

Does it still help? What about the "greenness" of it? If more of the copper is etched off, more metal will be recovered from the fab company's chemical vats. Or does the additional etch time and and acid required for clearing the board of copper outweigh the benefits of the additional recovered copper?

Looking at all of the boards we get through our assembly lines here, I can't really tell a general industry preference. It's hard to detect an internal plane visually and surface pours don't seem to be any more popular then the lack of them. So, I don't know what the world says.

Any thoughts on this? Anyone? Anyone?

Duane Benson

Unequal Pad Sizes, Take 2

I wrote a post not long ago about via-in-pad and unequal pad sizes as a cause of tombstoning and I received a question from Aaron about unequal pad sizes:

"In my designs, I have ground pours that directly connect to pads. So as an example, a cap that goes from vcc to ground would end up with one pad attached to the ground pour. Because of the solder mask expansion, the ground side pad will be noticeable larger."

This is a pretty common practice. I do it myself sometimes. The risk of tombstoning or other solderability issues relates to a couple of things. First, the smaller the part, the more critical all of this is and the more likely it will be for problems to crawl up. I'm assuming we're talking about SMT parts. Thru-hole parts can have some issues with copper pours, but not near as many as can SMT.

Pour-with thermal Pour-no thermalThe first issue is that the copper pour on one side will act as a big heat sink and may lead to tombstoning, or at least a poor solder joint on the pour side. If high current isn't needed, then use thermal pads. That will help. I would guess that with a cap like you're describing, high current isn't a requirement.

The other issue Aaron mentioned was the soldermask expanding on the copper pour and making the aperture size smaller then on the other pad. You can try to make soldermask defined pads on both sides. Then, in theory, the mask expansion should be close to the same on both sides. You can also make a larger mask opening on the side that goes on the pour so that after expansion, it will approximate the other pad size. The problem with this approach is that if you change board houses, you may not have the same amount of expansion. The best option might be a call to your PCB fab house for a chat about control of the mask expansion.

Also, if you do use thermal pads, as in the illustration, that might just solve the expansion problem right there. Most CAD packages have either a global setting to make all pads in pours thermal pads or a properties setting for each part that would make thermal pads as illustrated on the right above.

Duane Benson
Pour poor pitiful me into a picture of a pitcher