Issue link: https://iconnect007.uberflip.com/i/1408619
76 DESIGN007 MAGAZINE I SEPTEMBER 2021 1. SMT components on the flex material Placing surface-mount components on the flex circuit is possible by using selectively bonded stiffeners where required; several are shown in Figure 3. Copper on a flexible substrate is more susceptible to delamination than on a typical rigid board; consequently, surface mount pads require support, typi- cally using a coverlay overlap onto pads and vias. Enlarged pads can be used instead of a coverlay, which provides greater area on the pad to adhere to the laminate. Using both sup- port methods produces a pad with excellent adhesion. 2. Make pads larger than holes in coverlay Making pads larger than the access holes in the coverlay (Figure 4) can significantly increase bond strength while decreasing delamination possibility. is technique is similar to solder-mask-defined pads for rigid PCBs. With flex designs, the coverlay adds additional anchoring to the copper features. 3. Bend area conductor spacing Bend areas are another area that require careful design. e rule of thumb for conduc- tor spacing is 5 mm between the rigid board and the bend area of the flex circuit (Figure 5). Bends closer than this are much more suscep- tible to breakage. Also, without proper spac- ing, the coverlay under the rigid area can peel and expose copper. 4. Sharp trace angles at bend points ere is a second issue with bend areas relat- ing to trace direction. Flex circuit reliability and quality can be improved by ensuring that traces flow into the flexible circuit bend with little or no change in trace direction, also seen in Figure 5. If a change must be made in the direction of the traces in the bend, use curves instead of angled paths to reduce the chance of cracking the traces in the bend. 5. Conductor width Conductor width is also especially impor- tant. A safe rule-of-thumb for conductor widths is to design them at least five times as wide as they are thick. Our recommended practice is using the thinnest copper trace that will safely carry the intended signal and then adjust trace width accordingly. 6. Plane hatching Stress at the bend points can be relieved using a technique called plane hatching. While a honeycomb shape (hexagon) will alleviate the most angular stresses, any hatching will have a strain reduction when compared with that of a solid shape. 7. Pad fillets improve strength Pad fillets (example F in Figure 3) improve the yield and strength of flexible PCBs. ey should be employed in instances where the diameter of the pad exceeds the connecting trace width. You should also avoid acute angles at the interface between traces and pads with fillets to minimize the stress at the junction. 8. Interface region If a coverlay does not extend over the entire rigid area, the area is called an interface region as shown in Figure 6. is is where the flex and rigid components meet. Typically, the area extends about 1.2 mm from the edge of the rigid board and into the flex area for a com- bined 2.5-mm region. e interface region can be more fragile than the rest of the design, requiring special design considerations. ese include avoiding vias, mounting holes, slots, plated through-holes close to where flex and rigid join and designing the angle where traces enter rigid sections of the circuit to be anything other than 90 degrees. 9. Relaxed tolerance Tolerances for flexible circuits must be more relaxed than for rigid PCBs. e materials and