Flex PCBs: Coverlay and Soldermask are Not the Same Things

Figure: Flex PCB with Stiffeners and Coverlay Protection 

Flexible PCB materials offer versatility in modern designs for condensing form factors, removing connector assembly costs, and guaranteeing low-loss electrical connectivity between zones. However, designers must consider some key features when conceiving such concepts. One such item, sometimes misunderstood, is the flexible protective surface for flex PCBs known as coverlay.  

This material indeed does "the job" of soldermask in flexible PCBs, but it is different. Coverlay is made from a polyimide sheet material offering durability and consistent, unbroken circuit protection, which soldermask cannot guarantee while flexing. If coverlay is your primary protective layer, it behaves like a soldermask, providing openings for your pads wherever you need them. In Gerber view, you will be forgiven for thinking you are looking at soldermask openings. However, coverlay pad exposures are not done using photolithography like soldermask. This coverlay is a consistent film, typically around 25um thick, and kept in place by an adhesive. The pad openings are typically cut by a cutting tool before stackup assembly.  

This production process means protective bridges between pads are the first thing to go. Depending on your supplier, a usable cutting tool can only handle a minimum distance between cutting pins (approximately 450um between features). This has implications for solder, which can now travel farther away from pads along the tracks if conditions are right. See below the comparison image of a DFN using soldermask openings versus coverlay, which leaves all pads, diepads, and tracks completely exposed. This presents risks to your DFN soldering integrity, which may be insurmountable. The exposure can pose a manufacturing challenge even for standard rigid PCBs; however, you are bound to get problems with flex PCBs. Devices may even pass electrical tests but fail in the field after a few flexes. 

Remember that the distance between copper pads on small packages such as DFN is extremely low, in the order of 150um or so. The diepad-to-pad distance can be close to that also, circa 200-250um. Now these parts are not stationary during reflow and move about. We are boiling solderpaste flux, with outgassing and bubbling activity happening. The part will "hop around" while at a temperature in reflow until eventually finding a resting place. During this activity, it is difficult to guarantee the integrity and isolation of solder on each peripheral pad as the component moves above them. The term solder thieving is a known term in reflow defect analysis.  

Therefore, taking the extra costs and designing a rigid-flex concept with soldermask zones may be beneficial. But it depends on your circumstances, complexity, and component packages. Regardless, one must be aware of the coverlay vs. soldermask divide and its challenges in flex design. Take this post as a forewarning before you build a new project around a flex PCB and some new sensor or other small packages. Make sure to talk to both your PCB supplier and your manufacturing engineers about these risks.  

Could you raise any additional comments or points relating to flex? You may post them here.   

Let us use these forums as an area of discussion so that we can all grow and avoid potentially costly design mistakes.