Designer’s notebook
Component Footprint Differences between Rigid and Flex Circuits
Flexible printed circuits have unique requirements for footprints owing to the nature of their application.
Here is another lesson I learned the hard way: taping out an FPC (flex printed circuit) using the usual components and finding it doesn’t really work that way. Several things separate a rigid board from a flex. One of the main tenets behind the different design rules is reducing the risk of the circuit peeling up when it gets flexed. Even without continuous flexing, a flex circuit can be under tension where it is folded, twisted, spindled or mutilated.

Ah, but the flexible section is generally not where we install components. Normally, a stiffener covers part of the flex, and components are on the other side. Therefore, it is rigid, right? Not really. Most stiffeners used on flex circuits have a degree of flex to them. Flex stack-ups are intended to be as thin as possible; it’s one of their advantages. Even stainless-steel versions have some give. Many are made of FR-4 or another layer of polyimide, not all that stout.

In short, this means we want something more like a Class 3 footprint in that the maximum size pad is preferred. More area gives it more bite on the surface. A typical rule for flex is to use a fillet to taper to the line width of the traces. Any abrupt angles are stress-risers and need to be avoided. Round things off rather than squaring them.

These flex circuits also require greater tolerance for add-on layers. Solder mask, coverlay, stiffeners and silkscreen fall under this umbrella. Let’s break down each of these materials as they relate to the component footprint.

It’s black over black, but the coverlay openings are visible in this close-up of an FPC with a USB-C connector footprint
Figure 1. It’s black over black, but the coverlay openings are visible in this close-up of an FPC with a USB-C connector footprint.
FPC
Figure 2. FPC from Figure 1, as seen from below. Note the numerous openings for the slots and large holes, while the pin pattern is a mass opening for this stiffener.
Solder mask. As you would expect, there is a specific material to call out for solder mask on a flex circuit. It bends without breaking, up to a point. We usually expand the solder mask by 0.1mm (or 50µm on each pad edge) for a rigid board. The happy place for an FPC solder mask opening is four times that, unless you choose laser-defined geometry. The result is that a row of pins is very likely to have gang relief instead of individual mask openings. Low-volume soldering helps prevent solder bridging.

Coverlay. Kapton is the popular trade name for this polyimide material. It is pre-cut with different methods, depending on accuracy and production quantity. Whether stamped with a die or milled with a rotating cutter, specific primitive shapes, mostly circles and rounded rectangles, work best for the openings. There are more options when a laser is involved, but the creativity it enables comes at a higher unit price. Photoimageable coverlay is a slightly less accurate possibility for the odd shapes that cannot be done using CNC.

A good coverlay has an organic appearance. If you’re going with the crowd, the color you want is black (FIGURE 1). That has little to do with the component footprint, just a note that there are options to consider. The clearance is likely to be another 0.2mm beyond the already generous solder mask opening. Specific openings in the coverlay deserve a layer of their own in the PCB footprint.

Stiffeners. In most cases, the areas with a stiffener will have the coverlay end with a nominal overlap of the stiffener, although they are on opposite sides of the flex. A transition area where the edge of the stiffener, the coverlay and solder mask all meet is always staggered. The coverlay goes over the top of the solder mask to help it stay down. The stiffener underpins the whole transition area. This is a no-via and no-pad zone. This is one of those things that will stop a design from getting into fabrication, if not done correctly.

Many flex circuits are nothing more than a bespoke cable between two other printed circuit boards. They have connectors of some type, gold fingers, through-hole, surface mount or ZIF connectors with their interlocking pins. Each of these has a specific stiffener under it. That stiffener geometry should be added to the footprint for reuse.

Supported pads vs. non-supported pads. The FPC industry makes a distinction between pads that include a hole and pads that attach to the rest of the circuit only by a trace on the outer layer. The plated through-hole or microvia acts as an anchor that keeps the pad from lifting during high-temperature excursions such as soldering.

If the pad is hanging out by itself, it is in danger of delamination in those harsh assembly environments. In those cases, we like to add so-called spurs to the pad. These are also called tabs, flanges, fingers, anchors or whatever, but I think spurs is the most precise term. Get ready for some weird padstack shapes as they grow one or more extra stubs, er, spurs!

Silkscreen. Marking on FPCs can be hit or miss. I tend to miss the mark, even when being really conservative with text height, stroke width, and so on. No matter how far marking is placed from the part, the vendor will suggest moving it farther away. Forget about part outlines. Board-level marking may be all you can expect.

Most flexes are relatively simple from a design standpoint, so that’s a plus. The easiest way to mark these types of circuits may be with a handheld rubber stamp and ink pad. Rigid-flex is a different animal, at least for the rigid area(s), but I recommend keeping it simple when it comes to marking an FPC.

Wrapping it up. With these limitations, the rigid footprints in your library may not be applicable. An alternative for each symbol is recommended to reduce the number of technical questions from the vendor once the board tapes out. Speaking of vendors, the ones that specialize in flex circuits really want to engage you early in the design cycle for numerous reasons. The stack-ups have more variables, and processes require more give and take.

And that’s before accounting for the actual flexing, the ESD film, tear-stops, ground mesh and other esoteric attributes of the flex fabrication and assembly processes. Developing a specific library to go along with the unique design rules is a good first step toward success in the flexible circuit realm.

John Burkhert Jr. headshot
John Burkhert Jr.
is a career PCB designer experienced in military, telecom, consumer hardware and, lately, the automotive industry. Originally, he was an RF specialist but is compelled to flip the bit now and then to fill the need for high-speed digital design. He enjoys playing bass and racing bikes when he’s not writing about or performing PCB layout. His column is produced by Cadence Design Systems and runs monthly.