Contact our corporate or local offices directly.
As the name suggests, a flexible printed circuit is a pattern of conductors printed onto a flexible insulating film. Rigid-flex is the name given to a printed circuit that is a combination of both flexible circuit(s) and rigid circuit(s), as shown in the image above. This combination is ideal for exploring the benefits of both flexible and rigid circuits - the rigid circuits can carry all or the bulk of the components, with the flexible sections acting as interconnections between the rigid sections.
Flexible circuit technology was initially developed for the space program to save space and weight. It is popular today as it not only saves space and weight - making it ideal for portable devices such as mobile phones and tablets - it can also: reduce packaging complexity by substantially reducing the need for interconnect wiring; improve product reliability due to reduced interconnection hardware and improved assembly yields; and reduce cost when considered as part of the overall product manufacture and assembly costs.
Flexible circuits are normally divided into two usage classes: static flexible circuits, and dynamic flexible circuits. Static flexible circuits (also referred to as use A) are those that undergo minimal flexing typically during assembly and service. Dynamic flexible circuits (also referred to as use B) are those that are designed for frequent flexing, such as a disk drive head, a printer head, or as part of the hinge in a laptop screen. This distinction is important as it affects both the material selection and the construction methodology. There are a number of layer stackup configurations that can be fabricated as rigid-flex, each with their own electrical, physical and cost advantages.
Designing a flex or rigid-flex circuit is very much an electromechanical process. Designing any PCB is a three-dimensional design process, but for a flex or rigid-flex design the three-dimensional requirements are much more important. Why? Because the rigid-flex board may attach to multiple surfaces within the product enclosure, and this attachment will probably happen as part of the product assembly process. To ensure that all sections of the finished board fit in their folded location within the enclosure, it is strongly recommended that a mechanical mock up (also known as a paper doll cut out) is created. This process must be as accurate and realistic as possible with all possible mechanical and hardware elements included, and both the assembly-time phase and the finished assembly must be carefully analyzed.
Altium Designer also supports rigid-flex when designing the physical assembly board of a multi-board design. Refer to this article for more information.
Flex circuits are created from a stackup of flexible substrate material and copper that are laminated together with adhesive, heat and pressure.
The most common substrate is polyimide, which is a strong, yet flexible thermosetting polymer (thermoset). Examples of polyimides often used in the manufacture of flexible circuits include: Apical, Kapton, UPILEX, VTEC PI, Norton TH, and Kaptrex. Note that these are registered trade names, owned by their respective trademark holders.
The copper layer is typically rolled and annealed (RA) copper, or sometimes wrought copper. These forms of copper are produced as a foil and offer excellent flexibility. They have an elongated grain and it is important to orient this correctly in a dynamic flex circuit to achieve the maximum flexing lifespan. This is achieved by orienting the dynamic flex circuit along the roll (so the circuit bends in the same way the foil was coiled on the roll). The flex manufacturer normally deals with this during the preparation of fabrication panels. It only becomes an issue if the designer performs their own circuit panelization (referred to as nesting in flex circuit design). The copper foil is typically coated with a photo-sensitive layer, which is then exposed and etched to give the desired pattern of conductors and termination pads.
The adhesive is typically acrylic, and as the softest material in the structure, introduces the greatest number of manufacturing challenges. These include: squeeze-out, where the adhesive is squeezed out into openings cut into the cover layers to access copper layers; Z-axis expansion defects due to the higher CTE (coefficient of thermal expansion) of acrylic adhesive; and moisture out gassing due to the higher rate of moisture absorbance, which can result in resin recession, blow outs and delamination at plated through hole sites. Alternative adhesives and adhesive-less processes are available; these may be more appropriate in less cost-sensitive applications.
There are a number of standard stackups available for flex and rigid-flex circuits, referred to as Types. These are summarized below.
Single-sided flexible wiring containing one conductive layer and one or two polyimide outer cover layers.
Double-sided flexible printed wiring containing two conductive layers with plated through holes, with or without stiffeners.
Multilayer flexible printed wiring containing three or more conductive layers with plated-through holes, with or without stiffeners.
Multilayer rigid and flexible material combinations (Rigid-Flex) containing three or more conductive layers with plated-through holes. Rigid-flex has conductors on the rigid layers, which differentiates it from multilayer circuits with stiffeners.
The PCB editor is a layered design environment. The copper layers are separated by insulation layers. In a traditional rigid PCB, these insulating layers are typically fabricated using FR4 and pre-preg, although there is a range of materials available, each with properties that suit different applications. For a traditional rigid PCB, these copper and insulating layers exist across the entire PCB, so a single layer stack can be defined for the entire board area.
A rigid-flex design does not have a consistent set of layers across the entire circuit design; the rigid section of the board will have a different set of layers from the flexible section. Additionally, if the rigid-flex design has a number of rigid sections joined by a number of flex sections, there may be a different set of layers used in each of these sections. A PCB editor with a single layer stack cannot support this design requirement. To support this, the PCB editor's layer stack management system supports the definition of multiple stacks, as shown below.
Main article: Defining the Layer Stack
To support the need to define a different set of layers in different areas of the board design, the PCB editor supports the concept of multiple layer stacks. This is achieved by having an overall master layer stack that defines the total set of layers available to the board designer in this design. From this master layer stack, any number of sub-stacks can be defined, using any of the layers available in the master stack. Each sub-stack is defined and named, ready for use in the rigid-flex design.
The layer stack defines the board design space in the vertical direction, or Z plane. In the PCB editor, the board space is defined in the X and Y planes by the Board Shape. The board shape is a polygonal region of any shape, with straight or curved edges that lie at any angle that can also include cutouts (internal holes) of any shape. The board shape is a fundamental concept in the PCB editor. It defines the area available for design (i.e. where the components and routing can be placed) and all of the PCB editor's intelligent analysis engines, such as the design rule checker and the autorouter, operate within the boundaries of the board shape.
Note that there is a single, overall board shape for the entire circuit design, including rigid-flex. Within this board shape, any number of board regions can be defined by placing Split Lines to divide the board into separate regions. Split Lines are defined in Board Planning Mode (View » Board Planning Mode or shortcut key 1).The image below shows a board shape that has been divided into three regions by the placement of the two horizontal blue Split Lines. Use the links above to learn more about splitting a board into multiple regions.
Main Article: Defining Board Regions and Bending Lines
As mentioned, in a traditional rigid PCB the copper and insulating layers exist across the entire PCB, so a single layer stack can be defined for the entire board shape. For a rigid-flex design made up of a number of rigid and flex regions where each region needs a different layer stack, an alternative approach is needed. In the PCB editor, this is achieved by supporting the ability to assign a layer sub-stack to a specific region of the board shape. To do this, double-click on the region to open the Board Region dialog, then select the required Layer stack in the drop-down, as shown in the image below.
Main article: Defining Board Regions and Bending Lines
If a region has a layer stack assigned and that stack has the Is Flex option enabled in the Properties panel, Bending Lines can be placed across that region. Each Bending Line has a: Radius, Bending Angle and an Affected area width property, allowing them to be displayed in their folded state as they would be in a real-world situation.
The PCB editor includes a powerful 3D rendering engine, which allows the presentation of a highly realistic three-dimensional representation of the loaded circuit board. This engine also supports rigid-flex circuits, and when used in combination with the Fold State slider in the PCB panel, it allows the designer to examine their rigid-flex design in the flat state, the fully folded state, and anywhere in between.
To switch to the 3D display mode, press the 3 shortcut key (press 2 to return to 2D or 1 to return to Board Planning Mode). The board will be displayed in 3D. If the component footprints include 3D body objects that define the mounted component, these will also be displayed. In the image below, you can see that the board includes a battery and a battery clip.
To apply all of the Bending Lines, slide the Fold State slider in the PCB panel when set to Layer Stack Regions mode as highlighted in the image below. Note that the bends are applied in the order defined by their sequence number. Bending Lines can share the same sequence number; it simply means that those bends will be folded at the same time when the Fold State slider is used. The board can also be folded/unfolded by running the View » Fold/Unfold command (or by pressing the 5 shortcut).
Main article: 3D PCB Video
The ability to fold a rigid-flex design can also be captured as a 3D movie. It is very simple to do and does not require the use of movie key frames during the folding sequence.
Refer to the main article referenced above for a detailed description of how to make a 3D movie. As a basic guide:
The video below was created using this process. It has the two key frames described above, plus one additional key frame that was added at the end to hold the final position for a second.
Below is a summary of key design areas that must be considered when designing a rigid-flex PCB:
Typical suggested documentation requirements include:
Flexible Circuit Technology - Joe Fjelstad
Flex Circuits Design Guide - Minco Products Inc
Machine Design website:
Contact our corporate or local offices directly.