will be under maintenance from Friday, Oct. 3rd at 6pm (PST) thru Sunday, Oct 5th at 11pm (PST). login, registration, community posting and commenting functionalities will be disabled.
Home > Community > Blogs > PCB Design > customer support recommended flex pcb design features in allegro pcb editor
Login with a Cadence account.
Not a member yet?
Create a permanent login account to make interactions with Cadence more convenient.

Register | Membership benefits
Get email delivery of the PCB Design blog (individual posts).


* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

Customer Support Recommended - Flex PCB Design Features in Allegro PCB Editor

Comments(0)Filed under: PCB Layout and routing, PCB design, Allegro PCB Editor, PCB Editor, PCB, layer stacks, layout, "PCB design", routing, Allegro 16.5, PCB design", 16.5, group routing, application note, Appnote, Appnotes, Allegro 16.6, 16.6, 16.6 routing, Cadence, Cadence Design Systems

Flexible PCBs are used widely in everyday technology and electronics in addition to high-end, complex completed components. Two of the most prominent examples of flexible circuit usage are in hard disk drives and desktop printers. The following blog highlights the features of Allegro PCB Editor (Allegro) along with the Miniaturization option that provides a routing solution for flexible (flex) circuits.

Flexible Circuit Technology

Flexible (flex) circuit technology is used for assembling electronic circuits by mounting the devices on flexible plastic substrates, such as polyimide or transparent conductive polyester film. As the name suggests, these circuits are flexible in nature and are used in consumer products as well as in computing applications and military equipment.

Some basic forms of flex circuits are:

  • Single layer - This construction entails circuits mounted on a single conductor layer made of metal or conductive polymer, over a flexible dielectric film.


  • Double layer - In this construction, flex circuits are placed on two conductor layers. Here, fabrication may require to be plated through holes, as needed.

  • Multi layer - The construction of flex circuits spanning three or more layers of conductors is known as a multilayer flex circuit. These multiple layers may not be continuously laminated together throughout the structure and may have openings, if needed.


  • Rigid flex - This structure is a combination of flex circuits placed on rigid as well as on flexible substrates. These are laminated together into a single structure.   

Board Outline

Flex boards are versatile in shapes. CAD design software, such as AutoCAD®, can be used to create a board outline that can be imported into Allegro PCB Editor. Allegro PCB Editor can import IDX, DXF, and IDF files that contain the outline, cutouts, and other mechanical features that are critical to the design.


                                      CAD to BRD Translation 

Design Guidelines for Flex Circuits

Flexible-circuit designs not only face challenges similar to the ones rigid PCB designs face, but also some additional challenges. The very nature of a flex circuit is in its being able to bend and flex. This makes it as much as a mechanical device as an electrical one. This creates a special set of requirements unique to flexible circuitry.

Understanding how these requirements interact allows a PCB designer to create a flex circuit that balances the electrical and mechanical features into a reliable, cost-effective interconnect solution.

The guidelines used for designing flex circuits using Cadence Allegro PCB Editor are described in the subsequent sections.

Routing Consideration Using Route Keep Out

In general, users set up the cross-section for the maximum number of layers as per the design requirements.

Then a designer adds Route Keep Out areas as required for the cavity between Rigid and Flex or connectors. Included in the stack-up are many user-defined layers to represent the flex cover and masking layers. The designer may add a line or rectangle at the bend areas where traces are required to cross perpendicular.

                         Cover layers for rigid-flex design

An example layout requirement for a multilayer (6 layer) Rigid-Flex design -

        Example Layer Stack-up for rigid-flex design

Top and bottom layers are shield while inner layers are flex layers. There is a stiffener in the middle to strengthen the symmetry. The areas highlighted in red are cavities. It is recommended to place layer restricted Route Keep Out (RKO) in flex board areas to specify the cavity area and make a note for the fabricator on cavity requirements.

                               Route Keepout as Cavity

The designer can use the Z-copy command to copy the RKOs to the other layers where routing needs to be restricted. Placing a connector at the protruding flex Layer 2 or 5 can be controlled by editing the pads associated with the thru hole connector (Use the option of null in the Pad_Designer for the layers that are not relevant.)

Conductor Routing

Flex requires special considerations for routing due to its flexible nature and its versatility in shapes. Below are the routing capabilities from Allegro PCB Editor which can be employed for flex routing.

Multiline Routing

The flex-interconnect path generally spans across the flex section of Rigid-Flex design. The preparation entails testing multiple routes of specific widths and the respective conductor spacing as per the floor plan. Flex circuits mostly undergo potential reroute for the bus.

Using the Hug-Contour Option

Rigid-flex designs require curved bus lines. A flex board outline may also change during the design cycle. The ability to easily adjust the connect lines to the new form factor is critical.

The Multiline routing feature coupled with the hug-contour option lets the designer route multiple lines on the flex portion of the rigid- design in minutes instead of long hours based on traditional routing of one trace at a time.

              Example of multiline route abiding the route keepin as contour

New Slide Functionality for Arc Editing

With v16.6, a new slide functionality has been introduced. The slide command utilizes a move-intersect algorithm that delivers smoother and localized edits. This change simplifies the slide of the off-angle arc routing, and provides new options to improve efficiency. Note: The bubble mode is no longer allowed to wear down the arcs of an existing route.

Auto Interactive Convert Corner (AiCC) command

In v16.6, the Auto Interactive Convert Corner (AiCC) command has been introduced to improve efficiency in converting route corners in the Allegro design. You can interactively select nets, clines, or segments, for conversion to Arc, 45, or 90 degree corners.

Choose Route - Unsupported Prototypes - Auto Interactive Convert Corner.

AiCC can be run on existing Nets, Clines, or Segments

In v16.5, the glossing routine can be employed to convert 45- and 90-degree bends to arcs. It is useful for flex circuits because the resulting arcs may be time consuming to edit manually.

Refer to the AppNote for the detailed procedures on various routing methodologies discussed above, and also various other aspects that are not covered in the blog above.

Click here for the AppNote.

Note: The above link can only be accessed by Cadence customers who have valid login credentials for Cadence Online Support (


Naveen Konchada
Cadence Customer Support



Leave a Comment

E-mail (will not be published)
 I have read and agree to the Terms of use and Community Guidelines.
Community Guidelines
The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.