5 Traps to Avoid When Changing from Hand to Machine Assembly

In the past, it was usually pretty easy to find chips in both surface mount and through-hole packages. Somewhere in the past decade or so, component manufacturers stopped introducing through-hole versions of their newest chips as standard practice. In many cases, new components can only be found in tiny QFN (quad flatpack, no leads), or wafer-scale BGA (ball grid array) packages.

The maker community, never shying away from a good hack, found ways to work with many of these parts while still hand building. There are very few components used in the pro-design world that are still unusable by a creative DIY maker.

But what happens when a maker has a great design and wants to mass-produce it?

Sometimes the techniques that make things work when hand soldering, will completely break a machine assembly process. To cure that ailment, I’ve compiled five common traps to avoid when moving from hand to robotic assembly.

5. Consider moisture sensitivity. 
It may not seem logical, but plastic does absorb moisture. And, it doesn’t have to be dropped in the sink for it to happen. Just sitting around exposed to the air, plastic chips will absorb humidity. In a reflow oven, these parts can end up acting a bit like popcorn. The moisture turns to steam, and if it can’t outgas fast enough, may split the chips open. Often, the damage isn’t visible to the naked eye, but with show up as an unreliable product in the field.

When we DIY folks hand-build boards, we tend to open the component packages and then just let the parts lie around without giving thought to proper storage. If you are going to send your project off to be machine assembled, you can do two things with moisture sensitive parts.

First, order the parts when needed, not before, and keep the packages sealed. Alternately, you can send in parts that have been exposed to the air; if you inform your assembly house that the parts are moisture sensitive, and ask that they be baked prior to assembly. Prebaking will remove the moisture safely.

4. Don’t skimp on solder mask. Some board fabricators offer reduced prices if you order your boards without soldermask or silkscreen. That’s not a problem when you’re hand building — you can regulate the amount of solder by eyeball.

However, when a stencil is used to apply solder paste and the board is run through a reflow oven, the solder will spread back on the exposed copper traces. This may leave your parts without enough solder on the pins to create a reliable connection.

Solder mask may add a bit of cost up front, but will increase reliability and reduce cost in the long run. Creative choice of solder mask color can also add some personality to your boards.

3. Silkscreen is important too. Lack of sIlkscreen isn’t a reliability issue, but it can make accuracy of assembly more difficult to achieve. In a perfect word, the CAD files would tell the assembly machines exactly where each part is supposed to go and what angle and orientation it needs.

Unfortunately, we don’t live in a perfect world (who knew?). It’s far too common to have footprints with errors in them, or components with ambiguous marking, to depend on the CAD files alone. Clear silkscreen will help to ensure that any errors in the data are caught visually.

If you don’t want to clutter your PCB with reference designators and polarity markings, put the designators and any other important markings in the document layer in your layout software. Then, tell your assembly house to look on that layer for the information.

2. No need to fear surface mount. One of the easiest ways to ensure that a board can be hand-built is to stick with through-hole parts. But doing so puts many limits on a design, and rules out a lot of new technologies.

Little breakout boards — a small surface mount chip pre-mounted on a PCB, with hand-solderable headers — are available for a lot of new parts, but not all. That’s helpful, but they take up a lot of extra board real estate and cost more that the part alone.

If you’re hand building a prototype, or a small number of boards for your own use, go ahead use a breakout board. But, when it’s time to get a thousand built up to sell, re-layout your PC board to use the chip without the breakout board. Just don’t forget the bypass capacitors or any other required support components.

As a bonus, many breakout boards are open source, so you may be able study and use a proven schematic and layout for that part of your design.

1. No open vias in pads. QFNs and BGAs have pins/pads under the part, often completely inaccessible. That’s fine for a reflow oven, but what if you’re soldering it by hand?

A common hand-soldering practice is to put large vias in the pad. Fix the part onto the board with tape. Then, turn the board over and stick solder and a small tipped soldering iron through the via. By doing this, you can hand solder almost any leadless surface mount part.

You can probably guess that I’m going to tell you open vias in pads will not work with automated assembly. The solder will flow down the via and end up on the back side of the board. You may end up with shorts on the back side, and parts that fall off of the front side, or just don’t connect with all their pads.

If you use the open via hand solder technique, you’ll need to re-layout your board without any open vias in the pads before sending it for manufacture.

0. Go for it! It wasn’t that many years ago when the tools and services necessary to get an electronic product manufactured were so complex and expensive as to pretty much make it impossible for DIYers to turn a hobby project into a small business. Times have changed, and with those changes, the hardware startup is back — and within just about anyone’s reach.

Duane Benson
Breaker, breaker, one nine, clear the line, we’ve got boards to build

Electronics Manufacturing Files: What We Need

Manufacturing is all about taking data from you and delivering some good working circuit boards. Well, it can be just data — as in full turnkey — or data plus some parts and or PCBs, as in a partial turnkey or a kitted job. Regardless of whether you’re sending parts and boards, or having the us as the EMS buy everything, we need good data, and a lot of it.

That data are the difference between the working boards you want and need and a random jumble of expensive paperweights.

We need a bill of materials (BoM), the job specifications (which you give us by ordering and describing any special instructions on our website), and the CAD design files. Fab and assembly drawings are always a good idea too. A little extra time spent on the files sent reduces risk, and that’s a very good thing.

The CAD design files include Gerbers, a centroid (aka pick-and-place or XYRLS file), and intelligent CAD files, such as ODB++ or IPC-2581. In some cases, such as Eagle CAD, we can use the native CAD board file.

The ODB++ and IPC-2581 file formats are the future of electronics manufacturing. They come with more data, and more accurate data, than do Gerbers. If you can send either of these two, please do so. Even if you have those, still send us the Gerber files. Gerbers are the lowest common denominator, and provide a base that we and PCB fabricators can work from.

The Gerbers are a set of files used to create the various layers of the board. Each layer requires an individual file, so a six-layer board (six copper layers) will typically require at least 13 distinct files: one for each copper layer, top solder mask, bottom solder mask, top silkscreen, bottom silkscreen, the drills holes, and solder paste for the top, and bottom if the board has SMT parts on both sides.

The drill file is combined with the Gerber files to line up the via and through-hole component holes with the appropriate spots in the PCB. Then the pick-and-place file will tell the assembler where to put each component, what angle to place it at, and which side of the board it goes in.

Fab drawings hold a human-readable, often in PDF format, description of the board and any special instructions needed by the fabricator. The assembly drawing would be the same, but for the assembler.

Sometimes the parts are too densely packed for the reference designators and polarity marks to show up on the actual board, or for aesthetic reasons, the designer doesn’t want them on the board. In such cases, all that information would be put into a set of assembly drawings; PDF files showing all of the necessary reference information.

As of this writing, the ODB++ and IPC-2581 file formats aren’t universally accepted, but are getting more so all the time. Use of these new intelligent CAD output file formats helps to reduce the number of manual steps and human interpretation, and will eventually lead to better quality and faster manufacturing times.

Duane Benson
What do we need?
What does it really matter?
Matter converts to energy
E=(what we need)C2

Power Distribution – To Route, or to Plane PCBs

Power distribution on a PCB can come in a number of forms. The three most common methods are:

  • Route power and ground.
  • Use surface layer floods.
  • Use internal planes.

After component positioning, you’ll need to look at power and ground distribution. With a two-layer board, your options are limited to individually routing power and ground, or using a polygon fill, also called a flood or pour.





For simple low-speed layouts, it’s common to route power just like any other signal. You’ll typically use a wider trace, which you can set manually, or with design rules. Drawing a polygon in the board shape, and giving it the same name as your power or ground signals may make the job easier. Keep in mind though, that you can end up with parts of a ground plane disconnected from the rest of the board. This is called an orphan. Some CAD error checks will spot such a problem and some won’t.

I made that mistake not long ago, as describe in this blog post.

If you have a four (or more) layer board, common practice is to designate one of the internal layers for ground, and one for power.







Doing so can leave more room for signal routing, can reduce EMI, and can leave a cleaner-looking, easier-to-debug board. It also reduces the chances of having orphan ground or power areas, as I warned against in the prior post.

Duane Benson
Chocolate layer cake with coconut frosting will not help with EMI


Mistakes Were Made — Too Much Ground Isolation

I recently ran a batch of my Neo Pixel clock boards through the factory here. It’s an Arduino UNO-based design that I made for myself not long ago. It sports an Atmega328P, with bootloader, an FT231X USB chip, and a DS3231 real time clock (RTC) chip. Pretty standard stuff. It doesn’t even use small parts. All the passives are 0805 size. There’s nothing exotic here. So, where did I go wrong?

I also used my 3D printer to make a clock frame to hold this board and a 60-pixel ring of NeoPixels, from Adafruit. I found that with the micro USB connector on the top of the board, it’s a little awkward to plug in the USB cable, so I put pads for the connector on the back side of the board. Depending on exactly where and how the board will be used, the micro-USB, button switches, and clock backup battery can all go on either the front or back surface of the board.

Programming the bootloader worked as expected, so I assumed it was just a job well done. Except it wasn’t. When I plugged in the micro USB cable, the RX and TX LEDs flickered briefly, but the board wasn’t recognized by my PC.

Take a look at the back side of the PCB and see if you can find my mistake (spoilers after the photo).

I ran a 24 mil trace around the back side of the board to supply power to the NeoPixels. That’s not a problem, except that I closed the loop on that trace, and didn’t put a path for the ground to get across the trace.

Follow it around, and notice that the ground connections to the u-USB connector don’t go anywhere except to this part of the plane. Ugh.

Duane Benson
Cassini’s gone now.

QFN Center Pad Revisited

The QFN (quad flat pack, no leads) package can no longer be considered exotic. It was when I first wrote about it a decade ago, but not anymore. In fact, with the wafer-scale BGA, it’s one of the more common packages for new chip designs.

Not all QFNs come with an exposed metal pad underneath, but most do, and that can cause problems with reflow solder. The pad itself isn’t the problem, but improper solder paste stencil layer design can be.

The default stencil layer in the CAD library footprint might have an opening the full size of the metal pad. If that’s the case, modify the footprint so that there will be 50% to 75% coverage with solder paste (Figure 1). If you don’t, it may result in yield problems. With a 100% open area, the likely result is too much solder in the middle. The part will ride up, or float, and may not connect with all of the pads on the sides of the part.

Figure 1

Figure 1. The optimal QFN footprint will have 50% to 75% solder paste coverage.


Figure 2 shows a stencil with too large an opening in the center, a segmented paste layer in the CAD footprint, and the resultant segmented stencil.

Figure 2

Figure 2. Stencils shown with too large an opening in the center (left), segmented paste layer (center), and the resultant segmented stencil (right).


You may note that I said to shoot for 50% to 75% coverage and ask: “Well, is it 50% or 75%? What gives?”

True, that is a bit of ambiguity. Anything in that range should be fine for prototype boards, however. If the assembly is headed for volume production, work with the manufacturer to tweak the design for best high-volume yield.

The good news on this front is that many QFN manufacturers and parts library creators have taken notice. It’s far more likely now than it was 10 years ago to find a datasheet correctly illustrating this, and footprints created correctly. But, always check your footprints to make sure.

Duane Benson


Never Take Pin Numbering for Granted

Our all-things-about-electronics manufacturing standards body, the IPC, specifies the proper numbering order for most components. That’s a pretty nice thing that they do there, but it’s not always enough to prevent layout mishaps. Case in point a line of small PCB mount switches.

IPC calls out pin numbering for dual inline components, with pin one on the upper left (at zero degrees rotation), counting down, then over to the bottom right, and counting back up, as in the illustration below.

Given, that, it would be logical to assume that all dual inline components follow the same pattern. Logical, yes. Accurate, no. Multi-color LEDs, connectors and switches are some of the more common offenders.

In this particular switch, it’s not just a case of the numbering not following convention, it’s also different from one variant to another. I understand why. The switch isn’t changed between through-hole, top mount surface mount and side mount surface mount, but the leads have to be accessible from different parts of the package.

The following two footprints are from the same switch. One mounts on its side, and the other, standing up.

The pin one numbering doesn’t follow convention, nor does the numbering of pins 4 – 6. And, you may have also noticed that the two are top-to-bottom mirror images of each other. Ugh.

This is why my mantra is: Always check the datasheet. Always.

Duane Benson
Don’t take it for granite either, because granite is too heavy.


Components So Fragile, They Break Before Arrival

There are a lot of components that require special handling. Some days, “special” requirements seem more the norm than the exception. But, every now and then, we see something that puts even those special components to shame.

Not long ago, we received a parts kit that contained a component so fragile, that most of them didn’t survive the trip with the shipper. It’s a 10 x 9mm (well, actually 9.68 +0.00/- 0.08mm x 8.64 +0.00/- 0.08mm, to be precise) sensor that’s only 0.05mm thick. That’s 1/4 as thick as the diameter of the solder balls connecting it to the PCB.

The part has solder balls on the silicon, with no other packaging. The dice has to be that thin, as the light-sensitive area is on the other side. That doesn’t make for a very robust component. It would require special handling all around. Unfortunately, no matter how careful we might be, if they’re broken when we receive them, there’s not much we can do (other than take pretty pictures).

In taking these closeups, I noticed that the registration in ball placement isn’t all that great. In the image below, take a look at the ball on the left, second from the bottom, and the ball on the far right.

The datasheets call out all non-specified tolerances as +/-0.001mm. With these being 0.2mm diameter solder balls, I’d have to say this is way outside of that tolerance. I’m sure the part would have adhered to a decent board just fine, but if the PCB were off a similar amount in the opposite direction, you may very well have a problem.


Duane Benson
You could make a very tiny sundial out of this.
But, could you use the shadow parallax to calculate the distance to the sun?


What Makes a Good Fiducial?

Accountants may have a fiduciary responsibility, but that really has nothing to do with PCB assembly. Change the “ry” to a “ls,” however, and you get fiducials, which does have something to do with PCB assembly.

A fiducial is essentially an alignment mark for surface-mount assembly machines. High-volume assembly requires them to ensure accurate registration and parts placement. Low-volume assembly, like we do at Screaming Circuits, doesn’t necessarily require them. (Some low-volume shops do, so ask before assuming.) Even if they aren’t required, they still help and are always a pretty decent idea.

The basic idea, explained in this blog post here, is to create a non-reversal pattern with two or three fiducial marks on the board or panel. As you can see in the image above, the designer placed three fiducials around the board in a non-reversible pattern. (To protect the confidentiality of the board design, I obscured the circuit detail with this convenient robot head.)

In terms of the specific construction of a fiducial, two things are most important: contrast, and accuracy of position.

Contrast comes from it being bare copper – make it 1 to 2mm in diameter. Don’t cover it with solder mask. Make the mask opening 2 to 5mm larger than the copper.

The image on the left shows closeup detail. This particular fiducial mark uses a square cutout in the silk screen. Most use a round cutout, but the shape isn’t all that important. The copper pad should be round, though.

Making it out of copper gives the positioning accuracy. I’ve been asked why silk screen markings aren’t acceptable. Silk screen isn’t always registered consistently, and is therefore won’t ensure accurate alignment. Don’t use silk screen as a fudicial or positioning mark of any kind.

Again, they’re generally required for high-volume manufacturing. We (Screaming Circuits) don’t require them for low-volume, but some assembly houses do. Even when not required, they’re still a good idea.

Duane Benson
Fiducial on the roof is a long movie
But at least it stays in place


Let’s Talk about HAL – And Another Thing

A few days ago, I wrote about HASL PC board surfaces, explaining that it’s not an appropriate choice for small parts.

Look at the same PCB image I used the other day. You might not recognize it because before it was on the right, and today it’s on the left. Getting past the fact that I just insulted everyone’s intelligence, there is something else about this board that we don’t recommend.

I’ll give you 30 seconds to figure it out. I don’t have a stopwatch, so the 30 seconds is on the honor system.

This is a land for a 0.5mm pitch BGA. As I wrote before, HASL is not the right choice for BGAs, especially for those of the smaller pitch variety. The other problem with this board is in the pad layout.

These are solder mask defined (SMD) pads – the solder mask covers the outer part of the pad, so the solderable copper surface is determined by the size of the opening in solder mask, not by the area of the copper pad.

For BGAs 0.5 mm pitch and larger, we (and pretty much everyone else) recommend non-solder mask defined (NSMD). With a NSMD pad, the solder mask opening is larger than the pad. This leaves more copper area to adhere to, including the sides of the copper pad. It tends to be much more reliable.

The image to the right illustrates the difference. 

The left-most pad in the image illustrates an SMD pad, while on the right is an NSMD pad. The NSMD pad leaves a lot more surface area of the copper pad for the solder ball to grip on, including the sides.

BGAs with 0.4mm pitches might need either SMD or NSMD pads, depending on a number of circumstances. Read this blog information for a bit more on 0.4mm. When in doubt, look in the back of the datasheet.

Duane Benson
Question for physicists and mathematicians:
Should the last recursion in the Mandelbrot set land on Plank’s constant?
Show your work.



Let’s Talk about HAL – For Big Parts Only

The board surface names: HAL and HASL (hot air leveling and hot air surface leveling) refer to the same thing. They are interchangeable terms. With that out of the way, I’ll get to my point, which is that HASL is not the right surface for all applications.

Take a look at the photo on the right. This is a 0.5 mm pitch BGA land, using lead-free HASL. Don’t expect good results with this board. It’s a good quality HASL board. Even the bumps on the pads are not out of line for a HASL PC board. It’s not a defect. It’s the HASL works.

The catch is that, while the PC board is perfectly good, it’s not the correct board surface to use for all parts. HASL is fine for larger parts, but for small components, it’s archaic and not reliable.

BGAs require a flat surface (also called a planar surface). With the bumps common on HASL boards, the BGA won’t have a flat surface. The solder paste won’t adhere evenly to the pads. The BGA will probably slide off the pads before reflow. It may end up far enough off that it can’t self-center, as BGAs usually do.

The HASL pads won’t all have an even amount of solder left on the board. Some pads will have more, some less. When added to the solder paste, the pads with more solder may end up bridging.

All of the issues become even more severe as the parts get smaller. Wafer scale parts, 0.4 mm pitch parts, 0201 passives, and other similarly or smaller sized components are essentially incompatible with the HASL surface.

So, what do you do? Order your boards with immersion silver or ENIG. Both give a nice flat surface that BGAs like.

Duane Benson
Open thse Posd Basy Doors Hasl