Skip to main content

Component Footprint Differences between Rigid and Flexible Printed Circuits

Flexible Printed Circuits Have Unique Requirements For Footprints Owing To The Nature Of Their Application.

Here is another lesson that I had to learn the hard way. That is to say, taping out an FPC (flex printed circuit) using the usual components and finding out that it doesn’t REALLY work that way. There are a number of things that 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 part is generally not the part where we install components. There is normally a stiffener covering part of the flex and components are on the other side. Therefore, it is rigid. Right? Not really. Most stiffeners used on FPCs have a degree of flex to them. Flex stack-ups are intended to be as thin as possible as one of their advantages. Even the stainless steel ones have some give. A lot of them are made of FR4 or another layer of polyimide; not all that stout.

In short, this means we want something more like a class 3 footprint where the maximum size pad is preferred. More area gives it more bite on the surface. One of the typical rules for flex is to use a fillet to taper down 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 off.

The other thing about these flex circuits is that they require greater tolerance for the add-on layers. Soldermask, coverlay, stiffeners and silkscreen are all under this umbrella. Let's break down each one of these materials as they relate to the component footprint.


As you would expect, there is a specific material to call out for soldermask on a flex circuit soldermask on a flex circuit. It bends without breaking - up to a point.  We usually expand the soldermask by 0.1 mm (or 50 microns on each pad edge) for a rigid board. The happy place for an FPC soldermask opening is going to be 4 times that number unless you go with laser defined geometry. The result is that a row of pins is very likely to have a gang relief instead of individual mask openings. Low volume soldering helps in the prevention of solder bridging.


Kapton is the popular trade name for this polyimide material. It is pre-cut with different methods depending on accuracy and production quantity. Whether it is stamped with a die or milled with a rotating cutter, there are specific primitive shapes, mostly circles and rounded rectangles that 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 you could not do with a CNC method.

Figure 1. Image Credit: Author - It’s black over black but the coverlay openings are visible in this close up of an FPC with a USB-C connector footprint.

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


In most cases, the areas with a stiffener will have the coverlay end with a nominal overlap of the stiffener though they are on opposite sides of the flex. A transition area where the edge of the stiffener and the coverlay and soldermask all meet is always staggered. The coverlay goes over the top of the soldermask to help it stay stuck 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.

Figure 2. Image Credit: Author - Same as 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.

A lot of flex circuits are nothing more than a bespoke cable between two other printed circuit boards. They will have connectors of some type, gold fingers, through-hole, surface mount or ZIF connectors with their interlocking pins. Each of these would have 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 one that is attached to the rest of the circuit only by a trace on the outer layer. The plated through-hole or microvia both act as an anchor that keeps the pad from lifting during high temperature excursions such as soldering.

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

Figure 3. Image Credit: I-connect007 - Mickey Mouse ears anyone? Dangling copper features will benefit from tucking under the coverlay whether or not there is a hole involved but anchoring spurs are definitely necessary for so-called unsupported pads - those without holes.


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 has a suggestion to move 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 hand-held rubber stamp and an ink pad. A rigid/flex is a different animal, at least for the rigid area(s) but I have to recommend keeping it simple when it comes to the marking of 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 in order 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 with you early in your design cycle for numerous reasons. The stack-ups have more variables and the processes require more give and take.

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 design rules is a good first step towards success in the flexible circuit realm.

About the Author

John Burkhert Jr is a career PCB Designer experienced in Military, Telecom, Consumer Hardware and lately, the Automotive industry. Originally, an RF specialist -- compelled to flip the bit now and then to fill the need for high-speed digital design. John enjoys playing bass and racing bikes when he's not writing about or performing PCB layout. You can find John on LinkedIn.

Profile Photo of John Burkhert