FPC Prototype in Humanized Way

Quick FPC, Rigid-flex PCB prototype and PCB Assembly

Flex PCB Blog
Reflow Soldering PCB Temperature Curve Explanation
What is FPC
Special attention points for flexible circuit wiring
Multilayer PCB Stack-up Basics | PCB Knowledge
PCB Protection: Potting or Conformal Coating? | PCB Knowledge
FPCway: Specialized manufacturer of flexible printed circuit boards and rigid-flexible printed circuits
Future Trends of Flexible Circuit Boards
Rigid-Flex PCB Stack-up for Impedance Controlled Designs
Control Impedance Between Rigid PCB and Flex PCB
Flex PCB Reliability and Bendability
Normal Flex PCB Specifications
Flex PCB Polyimide Coverlay and Solder Mask
Flex PCB Boards and Connectors
About RA Copper and ED Copper
Introduction of Flexible PCB
5 Tips For Designing Flexible PCB
Advantages of FPC (Flexible PCB)
Evolution of the Flex Printed Circuit Board
Benefits of Using Flex Circuit Boards
Why Rigid-Flex PCBs are Economical?
Flexible PCB vs Rigid PCB
Development of Flexible printed circuit board (FPC) market
Traditional Manufacture Engineering of FPC Substrate
Development Trend of FPC Board
Flex PCB and the Manufacturing
About Flex PCB design
About Flex PCB and Assembly
How to Ensure Flex PCB Design Success
How to Select the Appropriate FPC Materials?
The Differences In Rigid PCB, Flex PCB and Rigid-Flex PCB
Flex-Rigid PCB Design Guidelines
Beneficials for Polyimide Flex PCB Boards
About Stiffener on Flex PCB FPC circuit Boards
PCB Surface Finish Comparison
Copper Thickness for FPC Boards
Interconnect Solutions for Flexible Printed Circuits and Etched Foil Heaters
Advantages and Disadvantages of Rigid-Flex PCB
About FPC Plating Process
About EMI shield design for Flex Printed Circuit Board
PCB Assembly Blog
How to solve the problem of PCB warping deformation after welding large copper bar?
About PCB Assembly
QFP and BGA and the Development Trend in PCB assembly
Why some components need be baked before reflow soldering
About Flex PCB Assembly
Manual Soldering in SMT Assembly Manufacturing Process
BGA Components and BGA Assembly
Quick Understanding for PCB Assembly Process
About SMT Assembly (Surface Mount Technology)
About THT Assembly (Through-Hole Technology)
About Reflow Soldering
PCB Assembly Inspections and Tests
Panel Requirements for PCB Assembly
About SMT (Surface Mount Technology)
FPC Research Blog
Preparation of FPC based on ultrasonic spraying method_4_Experimental Results
Preparation of FPC based on ultrasonic spraying method_3_Experimental Procedure
Preparation of FPC based on ultrasonic spraying method_2_Experimental Platform and Principle
Preparation of FPC based on ultrasonic spraying method_1_abstract
Research on Layout Design Method of Ultra-thin FPC_4_Analysis of Layout Design Methods
Research on Layout Design Method of Ultra-thin FPC_3_Analysis of Layout Design Methods
Research on Layout Design Method of Ultra-thin FPC_2_Analysis of Layout Design Methods
Research on Layout Design Method of Ultra-thin FPC_1_introduction
Research progress on polyimide FPC_2_the field of FPC
Research progress on polyimide FPC_1_Introduction
Analysis of Vibration Characteristics of FPCBs _4_Summary
Analysis of Vibration Characteristics of FPCBs _3_Finite Element Analysis
Analysis of Vibration Characteristics of FPCBs _2_Theory of Vibration Analysis
Analysis of Vibration Characteristics of FPCBs Under Random Vibration_1_Introduction
Design Methods for FPCBs_5_Practical Application
Design Methods for FPCBs_4_Electrical Circuit Design and Examples
Design Methods for FPCBs_3_Structure Design Method and Examples
Design Methods for FPCBs_2_Component Selection Methodology and Examples.
Research on Design Methods for FPCBs
Application of MPW technique for FPCBs _4_Summary
Application of MPW technique for FPCBs_3_Experimental results
Application of MPW technique for FPCBs_2_Experimental setup
Application of MPW technique for FPCBs_1_Principle of MPW
Application of FPCB in PC motherboards_4_ Results and discussion
Application of FPCB in PC motherboards_3_ Numerical analysis
Application of FPCB in PC_2_ Experimentation
Application of FPCB in PC motherboards
A Bus Planning Algorithm for FPC Design _4_Experimental result
A Bus Planning Algorithm for FPC Design _3_Proposed Algorithm
A Bus Planning Algorithm for FPC Design _2_Preliminaries
A Bus Planning Algorithm for FPC Design _1_Introduction

Impedance controlled circuits in a rigid-flex PCB design is a common requirement throughout the industry in a wide range of applications. Having Impedance control, however, does create an additional challenge for designs that have very demanding minimum bend requirements. 


In this blog post, we will review the design and construction specifics of some of the more common rigid-flex circuit board constructions that meet our customers' requirements: impedance-controlled circuit configuration and the impact on flexibility/minimum bend capability, line widths and spacings, materials, copper thickness, and common constructions.


Impedance Controlled Circuit Configuration 


By far the most common configurations are the 4 variations of the microstrip and stripline as shown below. These configurations address the needs of 95%+ of all flexible circuit designs that we manufacture.


Embedded Microstrip


Edge Coupled Embedded Microstrip


Symmetrical Stripline


Edge Couple Stripline


Of the two common configurations, the microstrip is the preferred configuration for the flex area of a rigid-flex design. It requires only two flex layers (1 signal layer + 1 reference plane layer) and uses a thinner flex core thickness. This combines to allow for the tightest possible minimum bend radius, which is often necessary to meet the packing requirements of the specific design. This configuration however does not provide shielding against EMI/RF on both sides of the impedance-controlled circuits.


The stripline configuration has the added benefit of providing shield on both sides of the circuitry, however, it has a negative impact on the minimum bend radius capability and flexibility. The required 3-layer construction (1 reference plane + 1 signal layer + 1 reference plane) adds significant thickness to the flex area. In addition, thicker flex cores are needed between the 3 layers to achieve the impedance values. This configuration should only be used if shielding on both sides is a design requirement. 


Line Widths/Spacing, Copper Thickness, And Materials 


Line widths and spacing, and the copper thickness of the flex layers interact to achieve the impedance values required. Thinner copper allows for a thinner line width/spacing and a thinner flex core thickness. This results in a thinner flex area, which will have the highest degree of flexibility and the tightest min. bend capability.


The preferred copper thickness is ½ OZ copper. Allows for a 0.002”flex core thickness for a microstrip configuration and 0.003” flex cores for a stripline configuration.


The following are typical line widths and spacings for the more common impedance values when using ½ OZ copper: 




If 1 OZ copper is required, usually due to a higher current carrying requirement on non-impedance lines, the above line widths are not valid as a 0.004” line width is below the manufacturable limit of 1 OZ copper. This requires the line widths/spacing as well as the flex core thickness to increase, which negatively impacts flexibility.


Polyimide flex materials are very well suited for impedance-controlled designs. The material is homogenous, has a low DK (3.2-3.4), is very uniform, and has tightly controlled thickness. Polyimide coverlays are also used to encapsulate the flex layers. 


Minimum Bend Radius Requirements 


All flex designs require the minimum bend requirements of the design to be identified and the materials and construction reviewed to ensure that the finished parts are mechanically reliable when installed. This becomes more important for impedance-controlled designs as the impedance requirement will always require a thicker flex construction. 


As an example, a standard construction 2-layer flex area utilizing a 0.001” flex core with ½ OZ copper and 0.001” coverlays results in a finished thickness of 0.006” after lamination. Thinner 1/2 mil flex cores and coverlays can be used to reduce the thickness down to as low as 0.004” if needed. An impedance-controlled microstrip configuration, with a 0.002” flex core, increase the flex thickness to 0.007”. A 3-layer stripline significantly increases the flex thickness further to 0.012” due to the added third circuit layer and the increased 2 x 0.003” flex cores.


2-layer standard flex PCB construction


2-layer thin-build flex PCB construction


2-layer microstrip flex PCB construction


3-layer stripline flex PCB construction


Common Rigid-Flex Constructions 


Rigid-flex constructions and configurations are available in a very wide variety. The number of combinations is too many to cover within this blog. The following constructions are some of the more commonly used for designs that have an average amount of circuit complexity. For more advanced designs, there are constructions available with higher rigid and/or flex layer counts. For these designs, we recommend to our customers to have a preliminary design review discussion with our engineering team to review the specific routing and bend requirements of the design and from this determine the optimum construction that will meet the design needs.


Application: Connector to connector microstrip impedance control. No active components. 


Impedance lines dropped down to the flex layers immediately adjacent to the SMT pads or straight out from PTH connector holes, eliminating need for external layer impedance lines. Additional flex layers available for microstrip configuration if circuit routing exceeds 1 flex layer. The second signal layer need not be impedance-controlled, which allows for second layer flex core thickness reduction and thinner flex section. This is also available with a stripline impedance configuration. It is typically limited to 1 signal layer to prevent excessive flex area thickness.


4-layer rigid-flex PCB microstrip construction


5-layer rigid-flex PCB microstrip construction


5-layer rigid-flex PCB stripline construction


Application: Active Component Area Rigid Areas. 


Active components on one or both rigid circuit board areas that also require Impedance controlled signal routing on external layers. Typically requires a minimum of a 6-layer configuration to allow for additional rigid area reference planes to be located within an effective distance of the external layers and allow for practical Impedance line widths. Flex layer area can be configured as either microstrip or stripline. Microstrip can have additional signal layer if required as per above 5-layer microstrip example.  


6-layer rigid-flex PCB stripline construction


7-layer rigid-flex PCB stripline construction




Impedance-controlled flexible PCB designs add the requirement of both thicker flex core layers and tightly controlled lines widths and spacing to meet the specific impedance requirements. For the flex areas of a rigid-flex circuit board design, this results in an increase in the flex area thickness, which may then impact the part’s ability to meet the min. bend requirements. 


These challenges can be addressed in most designs with a thorough design review and input from an experienced supplier. Please feel free to contact FPCway if you have any questions regarding the design of controlled impedance flexible circuit board.

Contact us

  • Email: sales@fpcway.com
  • Tel: 086 18576671093
  • Skype: Downey_PCB-PCBA
  • Address: No.12, Shapuwei Industrial Road
  • Songgang Street, Baoan District, Shenzhen

About us

  • Based in Shenzhen China, FPCway is professional at Flex PCB,
    Rigid-flex PCB and PCB assembly services
  • Flex PCB compliant ISO9001, ISO14001, TS16949, UL, RoHS.
    PCB Assembly compliant ISO9001, IATF16949, IPC-A-610E.
  • Our aim is "Humanized way to make Flex PCB". Choose us,
    you will have the best flex PCB and assembly partner.


© 2023-2033 FPCWAY All Rights Reserved