Flexi and flexi-rigid PCB's
Flexi and flexi-rigid PCB’s are now being used in place of traditional FR4 in a large number of different applications. Benefits include solving interconnecting problems, reduction of weight, reduction of space and reduced assembly costs. Flexible applications can be dynamic flexing (designed for flexing or stress over a period of time at elevated temperatures) or flex & stay applications (designed for flexing once and being secured into place).
Types of flexi and flexi-rigid PCB's
Single-sided flexible circuits are the simplest and there for cheapest. Consisting of a single conductor layer on a flexible dielectric film with the option of a coverlay or semi flexible solder resist (for some flex & stay applications). Parts of the flexible can be made more rigid by the use of additional stiffeners.
Double sided flexible circuits consist of two copper layers with a dielectric layer in between. Normally connected with plated through holes, with the option of coverlay’s or semi flexible solder resist (for some flex & stay applications). Parts of the flexible can be made more rigid by the use of additional stiffeners.
Multilayer flexible circuits consist of three or more copper layers with a dielectric layer in between. Normally connected with plated through holes, with the option of coverlay’s or semi flexible solder resist (for some flex & stay applications). Parts of the flexible can be made more rigid by the use of additional stiffeners.
Flex-rigid PCB’s consist of a mixture of flexible copper conductor layers on dielectric film & rigid copper material. Normally connected with plated through holes. Coverlay’s are applied to the flexible copper conductor layer & solder resist applied to the rigid areas.
Flexi and flexi-rigid PCB's guidelines and material specifications
Tie downs and teardrops
Through holes in flexible circuits should have tie downs. Tie downs are extra copper areas attached to the pad that are captured by the coverlay to anchor the copper pad to prevent delaminating between the copper and the base material. The adhesion of the copper on flexible material is lower than that of standard rigid material. Extra care must be taken when soldering flexible circuits.
Teardrops are the gradual transition from copper track to copper pad. This should be added to both through hole pads and surface mount pads to reduce stress points. This helps eliminate braking during flexing.
Coverlay is a flexible material applied to the outside layers of a flexi and flexi-rigid PCB’s to insulate the copper, this is normally a polyimide or polyester material. The coverlay is produced with a drilling or routing process which gives limitations to the shapes of openings. The simplest and most cost effective way is to have individual pads, if space allows. A minimum of 0.20mm distance is required between individual pads. The option of grouping pads is available if space is limited. The coverlay pad should be a minimum of 0.25mm larger than the copper pad.
Coverlay around surface mount pads can be routed but a radius will remain from the size of the router or a laser cut process can be used to reduce the radius. Semi flexible solder resist (for some flex & stay applications) can be applied instead of a coverlay. This enables any shape to be used with a minimum of 0.10mm distance between individual pads.
Flexi and flexi-rigid PCB's: staggered conductors
Staggering conductors (copper tracks) is recommended as this maintains the maximum flexibility of the circuits. I beam designs occur when conductors on both layers lie directly on top of each other. These increase the stiffness of the circuits fold areas and is not recommended.
Fold Lines and Bend Radius
Fold lines can be added to your design by using tick marks which can be added to either the copper layers or silkscreen layers. These ticks aid in bending your flexi PCB in a specific position. The bend radius of your flexible should be approximately 10 times the over all material thickness including copper. A gap of at least 1.28mm away from any plated through holes should be observed. Tracks should be radiused to help alleviate breaking during folding and bending. The track widths should not change in the bend areas.
Solid copper shielding is the most common method but does increase the rigidity of the flexible and should be included in the thickness to bend radius calculation. Crosshatched copper shielding helps to retain the flexibility of the circuit. Copper shielding can cover all or selective areas on one or both sides.
Often application require support in areas where connectors or components are applied. Most materials can be uses as a stiffener, the most common being FR4, polyimide or polyester with thickness from 0.050mm to 2.400mm. Stiffeners can be bonded using a high temperature pressure sensitive tape or a thermal setting adhesive. Holes in stiffeners should be 0.40mm larger than the hole in the flexible to allow for registration. The position of the stiffener should overlap the coverlay by a minimum of 0.75mm so there is no common ending. This will remove the potential for stress and cracking.
Base Materials for flexi and flexi-rigid PCB's
The information below is standard for most base materials but for more information visit our flexi materials page for more information.
Base material copper thickness of 5, 9, 18, 35, 70 and 105 microns are available on one or both sides. Base material polyimide thickness of 12, 25, 50, 75 and 125 microns are available, standards are 25 & 50 microns. Coverlay polyimide thickness of 12, 25, 50, 75 and 125 microns are available, standards are 25 & 50 microns. Adhesive thickness consist of 12, 25 and 50 microns. FR4 & polyimide stiffeners start from 0.050mm.