Screaming Circuits: Tips and tools

Via in Pad x 8

Via in 8 pin padsHere's an interesting via in pad case. On the one hand, the footprint is very symmetrical and clean looking. On the other hand, it has open vias in the pads.

At first glance, I thought this was a DIP footprint with extra long pads, but it's not. It's for an SMT part. Personally, I would have put mask between the pads. Looking at the rest of the board (not shown), the spacing between pads and mask is pretty wide, so there may be a good reason. I'm not sure though.

Definitely, though, I would not put the vias in the pads like that. Those open vias will cause solder to flow down to the other side of the board, make a mess there and leave the chips without sufficient solder.

Duane Benson
Sucking solder through a straw - or via

More Thermal Examples

Speaking of thermal relief... Here's an interesting example I ran across the other day.

Thermal relief can be a pain. If you've got a high current device, you may want more than just the thin little connections, one per side, that you get with thermals. You might feel the need for greater current capacity or you may need all the copper to distribute heat. You might have one pad, like in this image, that lands on a plane but not the other one.

In this particular board, the designer just made a few parallel traces coming out of the pad rather than one thick one.

Multi-via passive

The other side of this passive part sits right on the ground plane and has the standard thermals so the other reason this might have been done is to keep the amount of copper trace coming into the pad to be equal to that on the other side. It doesn't have exactly the same amount of copper going into both pads, but it's much close than if just one thin trace had been connected on the left pad.

Duane Benson
One thin trace rides away

Electrolytic Ambiguity

I've written about ambiguity a few times before, like this post about fiducials. But I'm not talking about the PC board today. I'm talking parts. More specifically, I'm talking about silk screen markings for your parts on the PCB.

CapacitorsDiodes have a lot of opportunity for ambiguity, as you can read here. There are many ways to mark parts, but fewer ways to clearly mark them. Take a typical electrolytic capacitor. It can be thru-hole, smt metal can, tantalum, or a few other form factors. The capacitor manufacturers aren't doing any of us any favors where markation is concerned.

Check out this image. Yikes! In all cases shown here, I've oriented positive on the left, which, according to IPC is pin 1. This is also the zero degree rotation for the centroid value. But, isn't it nice of those component manufacturers to put the identification bar on the positive side for tantalum capacitors and on the negative side for metal can electrolytics? Not!

So, how should you mark this in the silk screen on your PCB? For an electrolytic capacitor, the best approach is to mark the positive sided with a (+), plus sign. If you mark pin 1, with the number 1, it can easily be mistaken for the minus sign. If you mark the negative side with a minus sign, it can easily be mistaken for pin 1.

For a metal can capacitor, it is also acceptable to put the notched outline in silk screen. We still recommend that you place the (+) plus sign on there too.

Duane Benson
I'm just positive I put the negative right on the left

Fiddling with Fiducials again

I recently posted a note about fiducials but I didn't have any images. Here's a couple of examples:

IPC acceptable fiducialsThis first example shows what IPC would like to see. If this is an individual board, this would be it. If it were part of a panel, you would follow the same pattern on the panel rails and also put it on each individual board in the panel.

As I wrote in the earlier post, we don't require these, but it's always a good idea. You'll need them once you go into volume manufacturing anyway.

The next example won't make IPC happy, but it will make Screaming Circuits happy:

Also acceptable fiducialsIt only uses two fiducial dots, but it isn't reversible. Reversibility is okay for jackets, but not for circuit boards. Since one of the dots is offset, it can't be placed on the machine and recognized as correct in any way except in the proper orientation.

The important aspect of both of these examples is that they remove ambiguity. There can't be any uncertainty, which is good because uncertainty is your enemy. It's a subtle enemy. It might not bother you 99.9 times out of a hundred, but then, when you're not looking, it can strike. So, give a hoot and stomp out ambiguity.

Duane Benson
False data can act only as a distraction. Therefore, I shall refuse to perceive.


P3281577 smIt's pretty important to have unambiguous polarity markings and pin one markings printed on your PCB. In theory, for SMT parts, it really shouldn't matter; the centroid would take care of the placement orientation. But, you may have noticed that it's not a perfect world. It took me a while to figure that out, but I have finally concluded such.

It's not uncommon for the CAD library part to have the wrong zero degree rotation orientation The IPC specified location for pin one orientation Quad and BGA for square chips like QFPs, QFNs and BGAs is either the upper left or middle top. Check out our Centroid guide for more detail. If it's wrong in CAD, the centroid will be wrong as will everything downstream. That's why markings on the board are still important.

What do you do if your part is ambiguous though? This particular chip has three markings that could be interpreted as pin one indicators. At first glance, I'd assume it's the dot in the center top. It would match with the text. However, there is a white dot in the lower left that could be pin one indicator which would mean, in this case, the CAD library component had the incorrect zero rotation orientation.

Datasheets aren't always easy to find. This one is behind a registration wall. If you have a part like this, it's really helpful if you include some documentation (in electronic form) clarifying. I found the datasheet for this particular part and was able to confirm that it is correct as placed with pin one down in the lower left (90 degrees).

Duane Benson
Via via in the board,
what's the top on my PCB?

More CAD footprint woes

AT this point, I really shouldn't call them "woes." More like business as usual. I'm talking about the need to make custom footprints, or at leas modify footprints. Back in the old days, the only thing needed to make footprints was some copper pds, maybe plated through, maybe not. It was pretty rare to even need to make a custom footprint. Other than the occasional odd switch or relay, it was all done.

I really need to just get over it though. On the one hand, it seems like none-productive time; like I should be able to get right to schematicing and layouting. On the other hand, It's so common, I just need to see it as no different than any other routing task.

Starting at the top of my BOM, I have:

  • An MCU in QFN format - I modified a symbol and added a custom paste layer to the copper land
  • Two SOIC Mosfet drivers - I modified the symbol on an existing footprint
  • Some Mosfets in a PowerQFN package - Made a complete custom footprint
  • A Mosfet in SOT-23 package - Who hoo! I found a workable part in the library
  • Some Power Schottky diodes - custom copper land

Custom footprints

I have another Schottky, some TVS diodes, LEDs and a bunch of passives that came straight out of the library. It's certainly not everything that needs footprint work, but with so many variations of the more complex parts these days, it safe to assume that any SMT project will require a fair amount of library work. It's just the way it is.

Duane Benson
It's a pain but at least it's not as bad as 11811 has it

Thru-Hole Parts

Screaming Circuits uses machines to place surface mount parts; even if it's just one board. Thru-hole are a different story though. Way back in the cobweby section of the building, we do have a thru-hole part sequencing and insertion machine. Our volume manufacturing division still uses it on occasion, but it's just not efficient for small quantities, which is why thru-hole parts get hand inserted at Screaming Circuits. We have three options for soldering the parts into your prototype. We can hand solder all of the parts, we can send the board through our selective solder machine or we can send it through the wave solder machine. We'll pick whichever route makes the most sense based on quantity and configuration.

It's good that we can solder the thru-hole parts, but how, you might wonder, do we know where to put the thru-hole parts? The SMT has the centroid file to tell our machines where to put them. Thru-hole Thru-hole locationsbeing more of a manual process, we rely on visual data. If your silk screen markings are readable, we can used that as a reference. If the parts will only fit one way into one footprint on the board, then  it's not much of a challenge. Regardless, make sure that the polarity is clear for any polarized components.

Sometimes, though, there isn't enough room on the PCB for clear silk screen and parts will fit in a number of different places. That's where the assembly drawing comes in. This illustrates an example of a suitable assembly drawing. It's got your web order number in the image and all of the parts are clearly pictured and their locations clearly identified. If any of the parts are polarized, make sure you include that information as well. Send the assembly drawing as a .JPG or PDF file format in your ZIP file with the BOM, Gerbers and Centroid.

Duane Benson
It just goes to the back side of the board. It's not a wormhole going to another galaxy.
Or is it?

QFN Custom Stencil Layer in Eagle

It's been said over and over that you don't want to leave the solder paste opening wide open for a QFN center pad. 50 - 75% paste coverage will get you bets results. With full coverage, your QFN can end up floating too high and not connecting with all of the pads due to their significantly smaller aperture.

But hCustom paste layer 1ow do you create a custom paste layer? In Eagle, it's not terribly obvious, but it is easy. Open the part that you want to customize in the Eagle Library editor. Open up the package for that component. Now, select "i" on the left side and click on the center pad. You might need to turn off the "tcream" layer in order to select the pad. Custom paste layer 2

In the Properties dialog box, un check the check box for cream. That will get rid of the standard stencil layer. Now you can use the rectangle tool to add in stencil cut-outs as you want the. Make sure you set the layer for the rectangle to be "tcream" and remember that you are drawing the cut-outs of the stencil, not the blocked part.

Obviously it will be different for every CAD package, but the concept is the same. As is the need to do so.

Duane Benson
The Internet is weird.
There's actually a website for paste eaters.

BGA pads with Vias

Via eyeballs

No. This isn't a closeup of an owl face.

There is still some debate on how best to create a land pattern for a 0.4mm pitch BGA. We recommend soldermask defined pads at that pitch. But that's not really what this post is about. Although this land pattern uses non-soldermask defined pads which can encourage bridges. If you need to cross a river, encouraging bridges is good. If you're trying to make a board work, they are not.

In the case of the two BGA pads shown, I really doubt you would have to worry about bridging. That's because the solder ball would most likely be sucked off the BGA due to the capillary action of the via in the middle of the pad. You most likely wouldn't get bridging. You most likely wouldn't get any contact of any kind at all. This will not work.

Duane Benson
Hoot. Hoot.

Small Open Vias

Tiny vias in qfp pad Parts change and so do vias. Our standard policy here is that open vias in pads are bad. We from time to  time recommend ways to plug them. Generally, you have several options. Like this post shows. However, with vias in the pads of really small parts, those solder mask options will probably not work. Solder mask generally isn't put down with enough precision to cover holes on tiny pads, and further, the solder mask would probably mess with the clearance. On the left is an example of a small QFP with open vias in the pads. Those are some small vias.

So, if solder mask isn't going to work, what QFN center void open vias will? Filling and plating over them. That's what will work. You really only have two choices: fill and plate, or live with a bunch of voids under the part and solder slopped on the bottom side of the PCB. Here on the right are two illustrations representing the issue.

In the top half of the image on the right, I'm representing the vias with copper plugs and plated over at the board fab house. As with all parts of this sort, there may still be tiny voids. IPC and the manufacturer will have guidelines on the maximum allowable voiding. On the bottom, you see what happens with the vias left open. You get two problems: big voids and solder on the underside of the PCB.

Certainly there are some applications where this doesn't matter. That's why there is a second choice: "live with a bunch of voids and slopped solder." If you can't live with voids and solder slop, you have to bite the bullet and pay the extra for a PCB with filled vias. Board houses that do this have a variety of materials to use including copper, electrically conductive epoxy and thermal conductive epoxy.

Duane Benson
Please sir, may I have some more voids?
No! No voids for you!